Examples
This document was uploaded by user and they confirmed that they have the permission to share it. If you are author or own the copyright of this book, please report to us by using this DMCA report form. Report DMCA
Overview
Download & View Examples as PDF for free.
More details
- Words: 74,800
- Pages: 492
FEMAP Examples
Version 9.3
Proprietary and Restricted Rights Notice © 2007 UGS Corp. All Rights Reserved. This software and related documentation are proprietary to UGS Corp. All trademarks belong to their respective holders.
UGS Web:
http://www.femap.com
Customer Support Phone: Web:
(714) 952-5444, (800) 955-0000 (In US & Canada) http://support.ugs.com
Conventions This manual uses different fonts to highlight command names or input that you must type.
a:setup
Shows text that you should type.
OK, Cancel
Shows a command name or text that you will see in a dialog box.
Throughout this manual, you will see references to Windows. Windows refers to Microsoft® Windows 2000, Windows Me, or Windows XP. You will need one of these operating environments to run FEMAP for the PC. This manual assumes that you are familiar with the general use of the operating environment. If you are not, you can refer to the Windows User’s Guide for additional assistance. Similarly, throughout the manual all references to FEMAP, refer to the latest version of our software. Special note for customers using Windows Vista: FEMAP 9.3 is being released close to the same time as the initial release of Windows Vista. Currently, Windows Vista is an “unsupported” platform. Although we have tested FEMAP on Windows Vista with much success, there are issues with many graphics cards and drivers not being available for Vista at this time, which may cause issues in FEMAP.
FEMAP Examples Proprietary and Restricted Rights Notice 1. Introduction Introduction to FEMAP . . . Using the FEMAP Examples Guide The FEMAP Documentation Set .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. 1-1 . 1-3 . 1-5
Hardware/Software Requirements . . . Installation - Stand Alone . . . . Network Installation - PC . . . . Improving Performance (RAM Management) Memory Setting Guidelines . . . . Licensing Conversion Methods . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. 2-1 . 2-1 . 2-5 2-11 2-12 2-12
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 3-1 . 3-2 . 3-8 3-12
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 5-1 . 5-1 . 5-9 5-11
2. Installing FEMAP
3. Analyzing Buckling for a Bracket Importing the Geometry . . Meshing the Model . . . Applying Constraints and Loads Post-processing the Results .
. . . .
. . . .
. . . .
. . . .
4. Creating and Meshing a Solid Model Importing the Geometry . . Creating the Solid Part . . Creating the Slot . . . Creating the Bolt Holes . . Creating the Guide Boss . . Applying Constraints and Loads Meshing the Model . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
5. Working with Groups and Layers Differences Between Groups and Layers Using Groups . . . . . . Using Layers . . . . . . Using a Contour Group for Post-processing
. . . .
. . . .
6. Working with View Select and View Options Using View Select . Using View Options
. .
. .
. .
. .
4-1 4-2 4-4 4-8 4-10 4-16 4-18
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. 6-1 . 6-3
Post Processing Overview . . . . Generating Deformation and Contour Results Generating XY Plots . . . . . Using Results Displays in Other Applications
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 7-1 . 7-1 . 7-7 7-12
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
8-1 8-2 8-4 8-6 8-7 8-9
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
9-1 9-2 9-3 9-4
7. Using Post-Processing
8. Preparing Geometry for Meshing Understanding the Problem . Preparing the Geometry . . Creating New Boundary Surfaces Suppressing Features . . Meshing the Model . . . Applying Loads and Constraints
. . . . . .
. . . . . .
. . . . . .
. . . . . .
9. Repairing Sliver Geometry for Meshing Importing the Geometry . . Stitching the Surfaces . . Meshing the Model . . . Repairing Problem Geometry .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
TOC-2 Meshing the New Solid
.
10. Repairing a Mesh Importing the Mesh . Examining Free Edges Repairing Mesh Problems Meshing the Model .
. . . .
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
9-8
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
10-1 10-2 10-3 10-6
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
11-1 11-2 11-5 11-12 11-16 11-17
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
12-1 12-2 12-7 12-10 12-11
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
13-1 13-2 13-4 13-8 13-10 13-14 13-15
11. Analyzing a Beam Model Importing the Geometry . . Defining the Material and Property Meshing the Model . . . Applying Constraints and Loads. Analyzing the Model . . . Post-Processing the Results .
. . . . . .
12. Analyzing an Axisymmetric Model Importing the Geometry . . Meshing the Model . . . Applying Constraints and Loads. Analyzing the Model . . . Post-processing the Results .
. . . . .
. . . . .
. . . . .
. . . . .
13. Analyzing a Midsurface Model of a Welded Pipe Importing the Geometry . . Slicing the Model . . . Creating the Midsurface Model . Meshing the Model . . . Applying Loads and Constraints. Analyzing the Model . . . Post-processing the Results .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
14. Analyzing a Midsurface Model of an Electrical Box Importing the Geometry . . Creating the Midsurface Model . Meshing the Model . . . Applying Loads and Constraints. Analyzing the Model . . . Post-processing the Results .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
15. Direct Transient Analysis – Hinge Model Importing the Model . . . . . Creating the Transient Load . . . Defining the Transient Analysis Parameters Setting up the Analysis Set Manager . . Post-Processing the Results . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
14-1 14-2 14-8 14-10 14-12 14-12
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
15-2 15-6 15-7 15-10 15-12
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
16-1 16-3 16-5 16-12 16-14 17-2 17-5 17-8 17-10 17-13 17-14 17-16 17-18 17-19
16. Modal Frequency Analysis of the Hinge Model Importing the Neutral File . . . . . . Running the Normal Modes Analysis. . . . Creating Unit Load for Frequency Response Loading Running the Modal Frequency Response Analysis . Post-Processing the Results . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
17. Frequency Response of Tower with Seismic Excitation Importing the Model . . . . . Creating Function for Seismic Loading . Creating the Base Node and Rigid Connection Large Mass Method . . . . . Running the Seismic Analysis . . . Post-Processing the Results . . . Direct Method . . . . . . Running the Seismic Analysis . . . Post-Processing the Results . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
18. Random Response of the Hinge Model Opening an Existing FEMAP Model . . . . . Defining the Power Spectral Density Function . . . Creating Enforced Motion Loading - Large Mass Method
. . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. 18-1 . 18-3 . 18-7
TOC-3 Creating Enforced Motion Loading - Direct Method Setting the Random Response Parameters . . Creating a Group for Output Request needs . . Running the Random Response Analysis . . Post-Processing the Random Response Analysis .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
19. Generation of Response Spectra - Single Degree of Freedom model Creating the Model . . . . . . . . Creating the Dynamic Loading Function . . . Creating the Load . . . . . . . . Setting the Response Spectrum Generation Parameters . Setting up the Analysis Set Manager . . . . Post-processing - Response Spectrum Generation . .
20. Thermal Stress Analysis -
. . . . . .
. . . . . .
. . . . . .
Mounting Plate
Importing the Model . . . . . . . Creating the Thermal Boundary Conditions . . . Running the Steady-State Thermal Analysis . . . Post-Processing the Thermal Results . . . . Creating Nodal Temperatures from the Thermal Results Running the Thermal Stress Analysis . . . . Post-Processing the Thermal Results . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . .
. . . .
. . . .
. . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
19-1 19-3 19-5 19-8 19-10 19-12
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
20-2 20-3 20-7 20-8 20-9 20-12 20-13
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
21-1 21-4 21-8 21-9
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
22-1 22-2 22-4 22-5
. . . . . . . .
23. Temperature - Dependent effects - Circuit Board Opening an Existing FEMAP Model . . . . . Creating a Temperature Dependent Material Property . . Creating a Temperature Dependent Convection Coefficient (h) Running the Steady-State Thermal Analysis . . . . Post-Processing the Thermal Results . . . . .
24. Enclosure Radiation
Opening a FEMAP Model . . . . . Creating Materials and Properties . . . . Reversing the Element Normals . . . . Creating Radiation Emissivity and Heat Flux Loads Running the Steady-State Thermal Analysis . . Post-Processing the Thermal Results . . .
. . . . . .
. . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
23-1 23-2 23-5 23-8 23-9
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
24-1 24-2 24-6 24-9 24-14 24-15
25. Plastic Deformation of Rod - Nonlinear Material Creating the Nonlinear Material . . . . Creating the Property and Mesh . . . . Creating Loads and Constraints . . . . Running the Nonlinear Static Analysis with two cases Post-Processing the Results . . . . .
26. Gap Contact - Cantilever Beam Creating the Geometry . . . . Creating the Materials and Properties . Creating the Gap property and element . Creating the loads and constraints . . Creating Settings for Nonlinear analysis Running the Nonlinear Static Analysis . Post-Processing the Gap Contact Results
. . . . . . .
. . . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
25-1 25-5 25-7 25-11 25-14
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
26-1 26-2 26-6 26-9 26-11 26-13 26-14
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
27-1 27-3
27. Large Deformation - Cantilever Beam Creating the Geometry . . . Creating the Materials and Properties
. .
. .
. .
18-12 18-15 18-17 18-18 18-20
. . . . . .
22. Steady - State Thermal Analysis - Free Convection Opening an Existing FEMAP Model . . . Creating the Free Convection Boundary Conditions Running the Steady-State Thermal Analysis . . Post-Processing the Thermal Results . . .
. . . . .
. . . . . .
21. Steady - State Thermal Analysis - Circuit Board Importing the Model . . . . . . . . . . Creating the Heat Generation Loads and Thermal Boundary Conditions Running the Steady-State Thermal Analysis . . . . . . Post-Processing the Thermal Results . . . . . . .
. . . . .
. .
. .
TOC-4 Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Large Deformation Results
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
27-10 27-12 27-13 27-14
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
28-2 28-3 28-4 28-8 28-13 28-14 28-15
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
29-2 29-3 29-7 29-9 29-10 29-11
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
30-1 30-3 30-5 30-8
28. Slide Line Contact - Hyperelastic Seals Importing the Neutral File . . . . . Modifying the Material . . . . . Creating the Slide Line Property and Element . Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Slide Line Contact Results .
. . . . . . .
. . . . . . .
29. 3-D Contact - Plastic Clip and Base Importing the Neutral File . . . . . Creating the Contact (Slide Line) Element. . Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Slide Line Contact Results .
. . . . . .
. . . . . .
30. Large Deformation - Advanced Nonlinear (SOL 601) Importing the Neutral File . . . . . Creating the functionally dependent loads . . Running the Nonlinear Static Analysis . . Post-Processing the Large Deformation Results
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
31. Surface to Surface Contact - Advanced Nonlinear (SOL 601) Importing the Neutral File . . . . . . Creating the Contact Conditions. . . . . Creating the loads and constraints . . . . Running the Nonlinear Static Analysis . . . Post-Processing the Surface to Surface Contact Results
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
31-2 31-3 31-6 31-9 31-11
Importing the Geometry . . . . . . . Creating Connections . . . . . . . . Applying Loads and Constraints. . . . . . Meshing the Model . . . . . . . . Analyzing the “Glued Contact” Model . . . . Post-processing the Results of “Glued Contact” Analysis . Modifying the Connection Property . . . . . Applying additional Constraints for stability . . . Analyzing the “Linear Contact” Model . . . . Post-processing the Results of “Linear Contact” Analysis.
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
32-1 32-2 32-8 32-13 32-15 32-16 32-17 32-20 32-21 32-22
32. Analysis of a Simple Assembly
Index
1.
Introduction
This section introduces FEMAP and explains how to use the FEMAP Examples guide.
Introduction to FEMAP FEMAP is finite element modeling and post-processing software that allows you to perform engineering analyses both quickly and confidently. FEMAP provides the capability to develop sophisticated analyses of stress, temperature, and dynamic performance directly on the desktop. With easy access to CAD and office automation tools, productivity is dramatically improved compared to traditional approaches. FEMAP automatically provides the integration that is necessary to link all aspects of your analysis. FEMAP can be used to create geometry, or you can import CAD geometry. FEMAP provides powerful tools for meshing geometry, as well as applying loads and boundary conditions. You may then use FEMAP to export an input file to over 20 finite element codes. FEMAP can also read the results from the solver program. Once results are obtained in FEMAP, a wide variety of tools are available for visualizing and reporting on your results. With FEMAP you can: •
Import or Create Geometry
•
Build a Finite Element Model
•
Check Your Model
•
Analyze Your Model
•
Post-process Results
•
Document Results
Import or Create Geometry FEMAP can directly import geometry from your CAD or design system. In fact, FEMAP can directly import a solid model from any ACIS-based or Parasolid-based modeling package. If your modeling package does not use either of these packages, you can use the FEMAP IGES or STEP reader. If you are using I-DEAS, you can bring a single part into FEMAP by exporting a Viewer XML (IDI) file from I-DEAS. These files can be read and then stitched together to form a solid. This typically requires using one command. If you do not have CAD geometry, you can create geometry directly in FEMAP using powerful wireframe and solid modeling tools. Solid modeling directly in FEMAP uses the robust Parasolid modeling engine. You can build or modify solid models using the Parasolid engine, and then export the geometry out of FEMAP. This is very convenient if you need to export geometry to CAD packages that are Parasolid-based.
Build a Finite Element Model Regardless of the origin of your geometry, you can use FEMAP to create a complete finite element model. Meshes can be created by many methods ranging from manual creation, to mapped meshing between keypoints, to fully automatic meshing of curves, surfaces and solids. FEMAP can even work with your existing analysis models. You can import and manipulate these models using the interfaces to any of the supported analysis programs. Appropriate materials and section properties can be created or assigned from FEMAP libraries. Many types of constraint and loading conditions can be applied to represent the design environment. You can apply loads/constraints directly on finite element entities (nodes and elements), or you can apply them to geometry. FEMAP will automatically convert geometric conditions to nodal/elemental values upon translation to your solver program. You may even convert these loads before translation to convince yourself that the loading conditions are appropriate for your model.
1-2
Introduction
Check Your Model At every step of the modeling process, you receive graphical verification of your progress. You need not worry about making a mistake because FEMAP contains a multi-level undo and redo capability. FEMAP also provides extensive tools for checking your model before you analyze it to give you the confidence that you have properly modeled your part. It constantly examines input to prevent errors in the model, and provides immediate visual feedback. FEMAP also provides a comprehensive set of tools to evaluate your finite element model and identify errors that are often not obvious. For example, FEMAP can check for coincident geometry, find improper connections, estimate mass and inertia, evaluate your constraint conditions, and sum your loading conditions. Each of these methods can be used to identify and eliminate potential errors, saving you considerable time and money.
Analyze Your Model When your model is complete, FEMAP provides interface to over 20 popular programs to perform finite element analysis. You can even import a model from one analysis program and automatically convert it to the format for a different analysis program. The NX Nastran for FEMAP solver is a general finite element analysis program for structural and thermal analysis that is integrated with FEMAP.
Post-process Results After your analysis, FEMAP provides both powerful visualization tools that enable you to quickly interpret results, and numerical tools to search, report, and perform further calculations using these results. Deformation plots, contour plots, animations, and XY plots are just some of the post-processing tools available to the FEMAP user. FEMAP supports OpenGL, which provides even more capability for post-processing, including dynamic visualization of contours through solid parts. You can dynamically rotate solid contoured models with one push of your mouse button. Section cuts and isosurfaces can be viewed dynamically by simply moving your cursor.
Document Results Documentation is also a very important factor with any analysis. FEMAP obviously provides direct, high quality printing and plotting of both graphics and text. Frequently, however, graphics or text must be incorporated into a larger report or presentation. FEMAP can export both graphics and text to non-engineering programs with a simple Windows Cut command. You can easily export pictures to popular programs such as Microsoft Word, Microsoft Power Point, and Adobe Framemaker. You can export to spreadsheets, databases, word processors, desktop publishing software, and paint and illustration programs. These links enable you to create and publish a complete report or presentation, all electronically, right on your desktop. With support for AVI files, you can even include an animation directly in your Power Point Presentation or Word document. FEMAP also supports VRML and JPEG format so anyone can easily view results with standard viewers.
Using the FEMAP Examples Guide
1-3
Using the FEMAP Examples Guide The FEMAP Examples guide is designed to teach new users the basics of using FEMAP. It contains a number of examples that take you step-by-step through the processes for building and using an FEA model.
Working through the Examples As there are many different types of real analysis problems, there are different types of example problems shown here. Generally, you should start with the first example in chapter 3 and work through the examples sequentially. Some of the later examples focus on specific techniques that you may not use in your work (beam modeling, axisymmetric modeling, midsurfacing). However, we recommend that you work through all the problems because they may contain some commands or techniques that you will find useful. •
Analyzing Buckling for a Bracket
•
Creating and Meshing a Solid Model
•
Working with Groups and Layers
•
Working with View Select and View Options
•
Using Post-Processing
•
Preparing Geometry for Meshing
•
Repairing Sliver Geometry for Meshing
•
Repairing a Mesh
•
Analyzing a Beam Model
•
Analyzing an Axisymmetric Model
•
Analyzing a Midsurface Model of a Welded Pipe
•
Analyzing a Midsurface Model of an Electrical Box
•
Direct Transient Analysis – Hinge Model
•
Modal Frequency Analysis of the Hinge Model
•
Frequency Response of Tower with Seismic Excitation
•
Random Response of the Hinge Model
•
Generation of Response Spectra - Single Degree of Freedom model
•
Thermal Stress Analysis - Mounting Plate
•
Steady - State Thermal Analysis - Circuit Board
•
Steady - State Thermal Analysis - Free Convection
•
Temperature - Dependent effects - Circuit Board
•
Enclosure Radiation
•
Large Deformation - Cantilever Beam
•
Plastic Deformation of Rod - Nonlinear Material
•
Gap Contact - Cantilever Beam
•
Slide Line Contact - Hyperelastic Seals
•
3-D Contact - Plastic Clip and Base
•
Large Deformation - Advanced Nonlinear (SOL 601)
•
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
•
Analysis of a Simple Assembly
1-4
Introduction
The examples in this manual should help you learn the basic FEA modeling process, general FEMAP commands, and the FEMAP command structure. For a more complete description of the FEMAP interface and modeling procedures, see the FEMAP User Guide. For an in-depth description of all the commands in FEMAP, see FEMAP Commands.
Using the Examples In general, italicized text identifies items in the user interface. For example: File, Preferences tells you to pick the File menu, then the Preferences command. The Examples also include some graphics to help you identify user interface (UI) items. They include: UI Graphic
Meaning Pick an option from a cascading menu.
Menu
Pick an item from a pull-down menu on a dialog box.
Pick an item from a list.
Pick an icon.
Enter a value into a field on a dialog box.
Pick a button.
Pick a radio button.
Check an item on or off in a dialog box.
Pick with the left mouse button.
Pick with the right mouse button.
The FEMAP Documentation Set
1-5
Pick with middle mouse button if you have a three button mouse. Also can be the wheel of a wheel mouse.
Ctrl-A
Hold the Control key, then pick the letter key.
F5 key
Pick the function key.
The FEMAP Documentation Set FEMAP comes with a set of three printed manuals: FEMAP Examples, the FEMAP User Guide, and the FEMAP Commands reference manual. The FEMAP online help includes the contents of these manuals, as well as several additional books. The complete set includes: •
FEMAP Examples: Step-by-step examples for new users.
•
FEMAP User Guide: General information on how to use FEMAP, including an overview of the finite element modeling process. Also contains reference information for the FEMAP analysis program and geometry interfaces.
•
FEMAP Commands: Detailed information on how to use FEMAP commands.
•
FEMAP API Reference: Information on how to write your own applications that work with FEMAP.
•
What’s New: New features for this release.
When NX Nastran for FEMAP is installed, online help includes all of the above, as well as a full set of current NX Nastran documentation, to assist you during the solving portion of the analysis process.
1-6
Introduction
2.
Installing FEMAP
This section will help you install and start using the FEMAP software. This section contains information specific to getting started on a PC, which includes Windows 2000, Windows Me, and Windows XP. Special note for customers using Windows Vista: FEMAP 9.3 is being released close to the same time as the initial release of Windows Vista. Currently, Windows Vista is an “unsupported” platform. Although we have tested FEMAP on Windows Vista with much success, there are issues with many graphics cards and drivers not being available for Vista at this time, which may cause issues in FEMAP.
Hardware/Software Requirements There are no special hardware/software requirements for FEMAP beyond those imposed by Windows operating systems. There are many types of hardware that will allow you to use FEMAP. Proper choice of hardware, however, can often make the difference between frustration and productivity. Here are a few suggestions: •
Memory, RAM
•
Memory, (Hard Disk)
•
Graphics Boards
•
Browser
Memory, RAM You will need at least 32 Mbytes of RAM to run FEMAP. Furthermore, if you are going to use the solid modeling engines, 128 Mbytes of memory is required. Obviously, the more amount of RAM the better. Adding RAM can be one of the most cost effective means of increasing performance.
Memory, (Hard Disk) Required hard disk space is very difficult to estimate, but in general you will never have enough. Analysis results will be the main driver of any disk space requirement. Models are typically relatively small. A model with 1000 nodes and 1000 elements would typically be less than 1 Mbyte in size. Output from an analysis of that model, however, could be 5 Mbytes, 10 Mbytes or even larger, depending on the output you request. To estimate total disk space, you need to first estimate how many models you will have online simultaneously, the approximate size of those models, and the type of output you will request.
Graphics Boards Standard graphics adapters work very well with FEMAP. Specialized boards which contain support for OpenGL will provide increased graphical performance when dynamically rotating large, complex models. They also usually provide higher resolution and more colors, which make graphics easier to see and more realistic.
Browser To run the online help, you must have Netscape Navigator or Internet Explorer, version 4.5 or later.
Installation - Stand Alone This section describes the procedure that you should follow to install the stand alone (security device) version of FEMAP on your PC.
2-2
Installing FEMAP
Security Device Computer
FEMAP Printer
In order to run the Stand Alone (Security Device) version of FEMAP a Rainbow SuperPro Parallel Port (pictured on left) or USB Port dongle is required. In order for your PC to be able to see the dongle, a driver must first be installed. Installation of the driver requires Administrator privileges for your PC. During installation, if the current user has Administrator privileges, the installation program will automatically prompt for installation of this driver.
If the installer does not have Administrator privileges, someone with Administrator privileges will have to log in and install the driver manually. The driver installation program can be found in the /Rainbow directory of the FEMAP CD. On 32-bit Windows platforms, run CD\Rainbow\SPI722.exe. On 64-bit systems, run "CD\Rainbow\Sentinel System Driver\Sentinel Protection Installer\Sentinel Protection Installer 7.1.0.exe" It is highly recommended that you do not have any security devices attached to your computer while you are installing the driver. Once the driver has been installed, you can plug a USB security device directly into an open USB port and it should be recognized. For the Parallel Port security device, it is highly recommended that you shut your computer down and turn it off before installing the security device. After it is installed, turn the computer on begin using FEMAP.
Setup Program Execution Windows 2000/XP/Me 1. Log in to your computer as Administrator. As detailed above, this will make installation of the driver required to talk to the FEMAP dongle possible. 2. Insert the FEMAP CD into the drive. The setup should automatically begin within a few seconds. If it does not, manually run the SETUP.EXE program in the root directory of the FEMAP CD. Once setup is running you will see a license agreement. Assuming that you agree with the license agreement, press Yes to continue and select the directory where you would like to have the FEMAP program files installed. You will now be asked which type of installation to perform.
Setup Program Execution
2-3
Setup Type
Description
300-Node Demo
Installs the 300-Node demonstration version of FEMAP. This version requires no licensing, but is limited to very small models. It is intended for new users to try FEMAP and all its options.
Network Client
Network Client Installs the Network Client version of FEMAP. This setup is for use where FEMAP is licensed via the FLEXlm license management software. With the Network Client version of FEMAP, one machine on your network will be designated as the license server. The following "Network License Server" setup will have to be run on that mac
Network License Server
Installs the software required to run one computer on your network as the license server providing licenses to FEMAP client machines. The License Server machine can hand out as many licenses as you have purchased.
Stand-Alone
This is by far the most popular setup type used when installing FEMAP. It installs FEMAP for use with a Rainbow Parallel Port or USB dongle. If you have the dongle version of FEMAP, choose this setup type.
VisQ and Client and Server
VisQ is a free utility shipped with FEMAP. VisQ creates a client server environment where VisQ Server is installed on a computer that has access to FEA solver codes. VisQ Client machines can then send FEA input files to VisQ Server across the network. VisQ Server will run the analysis jobs in queue, and when each job is finished, the results are sent back to the client. For more information on VisQ, please see VisQ.PDF in the PDF directory under FEMAP.
After choosing your Setup Type, you will be prompted for the selection of additional FEMAP options, please choose any optional modules and components that you wish to have installed.
2-4
Installing FEMAP
Upgrading Your Security Device FEMAP dongles are shipped good for 30 days from the first time they are run. In order to remove the time limit from your new FEMAP dongle, or upgrade an older dongle or network license, you must contact UGS PLM's Global Technical Access Center (GTAC). In order to retrieve your FEMAP upgrade codes or your FLEXlm license file, you will need a GTAC WebKey account.
Obtaining a Webkey Account from UGS To request a WebKey account, access the web page; then provide the following information: https://plmapps.ugs.com/webkey •
Your Installation ID
•
WebKey Access Code
Your Installation ID is directly under the "sold to" information on your shipping order. For dongle-based FEMAP customers, your WebKey Access code is the unique portion of your FEMAP serial number, i.e. 3H-NT-1234, which is displayed in your current FEMAP in the Help - About dialog box, for this license as 820-3H-NT-1234, with the version information at the beginning of the serial number removed. If you have any problems determining your Installation ID, FEMAP Serial Number, or have trouble getting a WebKey account, please contact: Trish McNamara - [email protected] - 610-458-3660 x30, or Mark Sherman - [email protected] - 610-458-3660 x17
Obtaining Upgrade Codes or a new License File 1. Via the Web, using your WebKey Account -Upgrade codes or an updated license file can be e-mailed to you from the Customer Support (GTAC) web site http://support.ugs.com. Select the "License & Passwords" icon or select the "current license" option under the "License Retrieval" menu from the left side of the main GTAC screen. Select "Femap" as the Product. 9.00 as the Version, and fill in the LM Host with the unique portion of you FEMAP serial number (3H-NT-7878 in this case), or for FLEXlm network licenses, fill in the Ethernet address of your FEMAP license server. Your license will be e-mail to the address supplied during WebKey registration.
2. Via the Phone - You can call GTAC at 714-952-5444 (US and Canada residents may use 800-955-0000) and enter option 1, 1, for your CSR or option 1,2, for Software Product Delivery (SPD). You should then request a copy of the license upgrade for a specific Installation ID and serial number or Ethernet Address. For dongle versions of FEMAP, the information returned to you to upgrade the dongle will be in the form of two case insensitive alpha numeric codes. They will appear something like:
Access Code 1: 08aeca3f0f52639179 Access Code 2: 362ff63c3426d943
Use the Help, About command, then click the Security button. Cut and paste (to avoid errors) or type these two codes in to the appropriate fields and press OK. The FEMAP dongle is an EPROM, and these codes are used to update the memory of the dongle. Once these codes have been entered, you will never need to enter them again,
Network Installation - PC
2-5
with changes made to the memory of the dongle, they will either be useless, or simply write the same thing to memory again.
Network Installation - PC The “Network Client” version of FEMAP utilizes the FLEXlm License Manager software from Globetrotter Software Inc. This licensing approach requires some software to be installed on a server machine and other software to be installed on one or more clients. The clients then request and obtain licenses from the server. In a simple situation, both the client and server could be the same computer, but more likely they are different systems connected by a network.
Obtaining a License File License files are obtained through the same procedure as defined above for getting the upgrade codes for a dongle license. Call GTAC, or use your WebKey account to request your FEMAP license file. The only difference in Network Licensed FEMAP is that you need to enter the LMHostID (Ethernet Address) of your license server when prompted instead of the FEMAP Serial Number. When you receive your license file information, you need to extract just the valid FLEXlm license entries, and copy them into a file called "license.dat". Please make sure that your license.dat looks something like the one show below. For FEMAP, you will have one SERVER line, one DAEMON line, and one or more FEATURE lines depending on how many options you have purchased with your FEMAP. A couple of things to make sure of: 1. Make sure that the entry immediately following the word "SERVER" is the name of the license server where you are installing the license server software. If it is a temporary name, i.e. ANY, or THISHOST, change it to the correct machine name. This is one of the two things in the license file that you can change. 2. Make sure that the third entry on the SERVER line matches the LMHostID of license server. This number is the key to the whole license file. If this does not match the LMHostID of the license server, then the licensing will not work. 3. The "DAEMON esplmd" line calls out the actual programs that hands out FEMAP licenses. If you have installed all the license server pieces in the same directory, it is fine as is. If the esplmd.exe program is not in the same directory as LMTOOLS.EXE, you will have to edit this line to tell LMTOOLS.EXE where to find it. This is the other part of a license file that you can change. SERVER PHLF10 00095b8e20ef DAEMON esplmd FEATURE femap esplmd 9.20 18-may-2007 1 0588B50324A5 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapthermal esplmd 9.20 18-may-2007 1 DBB2754C3B21 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapadvthermal esplmd 9.20 18-may-2007 1 7033101A44B2 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapflow esplmd 9.20 18-may-2007 1 0F1D6AB8AE56 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_basic_fep esplmd 9.20 18-may-2007 1 EE2DC8632354 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_nonlin_fep esplmd 9.20 18-may-2007 1 861F50768DA3 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_dyn_fep esplmd 9.20 18-may-2007 1 8ECB283B0927 \ VENDOR_STRING=920-FX-NT-20ef0001762070000
License Server This section provides instructions on installing the network license manager and configuring your server.
2-6
Installing FEMAP
Installing the FLEXlm License Manager To begin the server installation, simply insert the FEMAP CD and allow it to AutoRun, or choose setup from the CD. When asked for the type of installation that you want to perform, select the "Network License Server" setup type. Once FEMAP has installed the software, copy your license file (usually called "license.dat") to the same directory where you installed the license server components.
Configuring the FLEXlm License Manager You can run the LMTOOLS program, from the FEMAP entry on your start -> All Programs - FEMAP v9 FLEXlm Tools, or manually run LMTOOLS.EXE from its installed directory.
Once LMTOOLS is running, select the "Config Services" Tab.
Fill in a Service Name, specify a path to the lmgrd.exe file (a required FLEXlm component) that can be found in the installation directory, and specify the path the license file. Finally, check the "Use Services" option, and then the "Start Server at Power Up". Press the "Save Service" button.
Answer "Yes" to:
You must start the license server manually the first time, press the "Start/Stop/Reread" tab.
Configuring the FLEXlm License Manager
2-7
Select the FEMAP service that you just created, and press the "Start Server" button. At this point FLEXlm will be handing out FEMAP licenses on your network. To verify that everything is working fine from the license server standpoint, press the "Server Status" tab.
Press the "Perform Status Enquiry" button and the text window will be filled with status information about your FLEXlm license server. In the text window you will find information about how many licenses are available, and once user start checking out licenses, how many are in use.
2-8
Installing FEMAP
Configuring Network Client Machines Once your network license server is up and running, configuring FEMAP Network Client machines is very easy. Make sure that FEMAP is installed on the local machine using the "Network Client" setup type. To configure client machines to access the network license: You have two options for telling network client machines how to find licenses on the license server: 1. Place a copy of the "license.dat" file in the FEMAP directory on the client machine. FEMAP will extract the name of the license server from the license file, and check out a license and run. The only drawback to this approach is that you must remember to update every copy of the license file when you receive a new one from UGS (updates, licensing changes, etc.). To avoid this problem, you can type in the full network path to the License File in the "License File" field used below for HostName/IP Address location of the license server. 2. Tell FEMAP the name or IP address of the License Server. a. Start FEMAP b. Go to Help - About - Security c. In the "License File" field, enter the name of the license server, preceded by an ampersand. In the example below, FEMAP is told to check out licenses from a network machine named PLSRV2: d. In order for this machine name approach to work, the client computer must be able to see the license server computer via TCP/IP networking. To verify this, you can open a Command Prompt and ping the license server. In this case, one would type "ping PHLSRV2". The ping command will let you know if it can talk to the machine name indicated. If the client computer cannot find the license server by its name, you can also enter the IP address of the license server, preceded by an ampersand and licensing should also work.
Monitoring Network Usage In a multi-user environment, sometimes you will not be able to get a license simply because all available licenses are in use. You can find out who is using licenses, which computers they are using and when they started their license simply by going to Help, About, and pressing the Security button. At the bottom of the dialog box you will find information that will give you this information. If you fail to get a license because none are available, you will not be able to work in FEMAP. You do not however, have to leave FEMAP. You can simply stay there and periodically try a command. Whenever a license becomes available it will be assigned to you and your command will succeed. If there are still no licenses available, you will simply get a message that says try again later.
Errors Starting FEMAP Security Device Not Found Symptom: You see an error indicating that the security device cannot be found. Resolution: Go to Section , "Security Device", and confirm all steps have been followed. Try to run FEMAP again.
Errors Starting FEMAP
2-9
Choose Server or File Symptom: If you are attempting to start a network client and see the Error dialog box from FEMAP, FLEXlm cannot find a valid license file. Resolution: Press Cancel in this dialog box. Pick Help, About, Security to define the location of the license file, as instructed above in Section , "Configuring Network Client Machines"
Unable to get license message:
LM_LICENSE_FILE environmental variable error:
This error will ONLY occur when the environment variable LM_LICENSE_FILE has been set. For example, this environment variable may have been set by another application for licensing purposes. Be careful when removing or altering this environment variable as it may cause other applications to no longer function properly.
Other Error Messages Symptom: If you receive an “Unable to allocate Scroll Buffer File” error or have any other difficulty starting FEMAP where abnormal termination occurs, you either do not have enough disk space, or your Windows TEMP is not set to a valid, accessible directory. Resolution: You may either change your Windows TEMP directory environment variable, or specify a path for the FEMAP scratch files (which default to the Windows TEMP directory set by the environment variable) to a valid directory. This and all other FEMAP preferences are stored in a file called femap.ini that is typically located in the FEMAP executable directory. You will have to create this file or modify it to include the appropriate lines as shown below: DISKMODELSCR=C:\FEMAP92 DISKLISTBUFF=C:\FEMAP92
2-10
Installing FEMAP
where C:\FEMAP90 can be any valid path. The DISKMODELSCR, DISKUNDO, and DISKLISTBUFF parameters are case sensitive, and must be defined exactly as above. Once you make these changes and FEMAP starts, you can use the File, Preferences, Database command to modify this path.
Starting FEMAP There are several command line options to launch FEMAP. The simplest method to launch FEMAP is to create a shortcut for FEMAP on your desktop and double-click the icon when you want to launch FEMAP. This will use the command line contained under the shortcut to launch FEMAP. You can modify this command line by right-clicking on the FEMAP icon, selecting properties, and changing the command line option on the shortcut. The command line will contain the executable (and its path). After the femap.exe, there are several options which may be used to determine the mode in which FEMAP will operate. A list of these command line options are provided below. c:\femap93\femap.exe [-R] [-NEU] [-NOSPL] [-D dxf_file] [-N neu_file] [-PRG program_file] [-SE Solid Edge_File] [-L port] [-SAT sat_file] [-XMT x_t file] [-SCA scale_factor] [-IGES iges_file] [model_file or ?]
where all of the arguments in [ ] are optional command line parameters. They are: The remaining parameters can be specified in any order. -R
Read Only Mode. With this option set, the Save, Save As and Timed Save commands are disabled. You will not be able to save changes to any model you access. All other commands remain active. Any changes you make will be made in the temporary scratch file, and will be lost when you exit FEMAP.
-NEU
Automatically writes a neutral file with the same name (just .NEU extension) as your .MOD file every time you save a model. In addition, when you open a model, if a neutral file exists with a newer date than the model, it will be read.
-NOSPL
Starts FEMAP without the splash screen.
-D dxf_file
This option automatically reads the specified DXF file when you start FEMAP. Make sure you leave at least one space between the two arguments.
-N neu_file
This option automatically reads the specified FEMAP neutral file when you start FEMAP.
-PRG program_file
This option allows you to run a specified FEMAP program file (*.PRO or *.PRG file) when FEMAP is started.
-SE Solid Edge_file
Automatically creates a new FEMAP file and calls the File, Import Geometry command to read the Solid Edge part file (*.prt file) or assembly file (*.asm file). When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box, which will contain the title of the solid model file contained in the SAT file.
-L port
Specifies the parallel port where the FEMAP security device has been installed. This is not typically needed unless FEMAP has difficulty accessing the device. If you want to attach the security device to parallel port 1 (LPT1:), use -L 1, for parallel port 2 (LPT2:) use -L 2. If your system is non-standard, or uses some other parallel port convention, you can specify the actual parallel port address. For example, if your parallel port was at address 03BCH (hexadecimal), you would convert the address to a decimal value, in this case 956, and specify -L 956. If you need to specify the -L option, you can change the default command line associated with the FEMAP icon on the Desktop by selecting Properties. First, right-click on the FEMAP icon. Then choose the File, Properties command (or press Alt+Enter). Move down to the command line option, and just add the appropriate -L options. From then on FEMAP will look for the security device on the specified port.
Improving Performance (RAM Management)
2-11
-SAT sat_file
Automatically creates a new FEMAP file and calls the File, Import Geometry command to read the ACIS solid model file *.SAT file [sat_file]. When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box, which will contain the title of the solid model file contained in the SAT file.
-XMT xmt_file
Automatically creates a new FEMAP file and calls the File, Import, Geometry command to read the Parasolid solid model file *.X_T file [xmt_file]. When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box which will contain the title of the solid model file contained in the X_T file.
-SCA scale_value
This option is used in conjunction with the -XMT and -SAT to specify a scale factor for the solid model. If this option is used, FEMAP will automatically import and scale the solid model. The Solid Model Read Options dialog box will not be shown.
-IGES iges_file
Automatically creates a new FEMAP file and calls the File, Import, Geometry command to read the file [iges_file]. When you use FEMAP with this command option, you will see the IGES Read Options dialog box, where you can specify options for reading the file.
model_file
Normally FEMAP will start with a new, unnamed model. If model_file is the filename of an existing model however, FEMAP will start using that model. If the file does not exist, you will see an error message, and FEMAP will start a new model with that name.
?
If you add a question mark to the command line instead of specifying a model name, FEMAP will automatically display the standard file access dialog box and ask you for the name of the model that you want to use. If you want to begin a new model, just press New Model or the Escape key. When you want to work on an existing model, just choose it from the dialog box, or type its name. You should never specify both the ? and model_file options.
Improving Performance (RAM Management) To improve FEMAP performance on Windows personal workstations, you should modify the default settings that FEMAP uses to manage RAM. For more details on this procedure, see Section 2.6.2.5, "Database" in FEMAP Commands. To access the internal FEMAP memory management system, follow the procedure below: 1.Choose the File, Preferences command and click the Database tab. 2.Change Cache Pages and Blocks/Page in the dialog box. 3.Set Max Cached Label to a number that is higher than any entity you will create in your model file. This sets aside a small portion of memory that stores all of the IDs in FEMAP. 4. Select OK The total amount of memory that FEMAP can allocate is the product of the Cache Pages, Blocks/Page, and 4096 bytes/ block. For example, with the values shown, 12000 x 2 x 4096 will allow FEMAP to access just under 100 Mbytes of RAM and use entity ID’s up to 6,000,000. Note: You should never allow FEMAP to allocate more than the physical memory of the machine. The internal memory management (swapping) in FEMAP will allow the program to run much faster than Windows memory swapping. Therefore, you should set the Cache Pages and Blocks/Page at a level which is comfortably below the physical memory of the machine. Also, to optimize performance, you should always increase Cache Pages (max 15000) to its limit before increasing Blocks/Page.
2-12
Installing FEMAP
Memory Setting Guidelines The following figures are provided as a starting point to improve performance. Operating System
Installed RAM (Mb)
Windows 2000, Me, 64 XP 128 256 512 1000
Cache Pages 6000 8000 12000 15000 15000
Blocks/Page 1 2 3 5 11
Actual performance will vary depending upon other concurrent applications and model specifics. It is best to increase Cache Pages to 15000 before increasing Blocks/Page. Note: For best performance, you should have enough physical RAM to load the entire model file into memory. For example, if you expect your model files to be a maximum of 100 Mb, then you would want FEMAP to allocate at least 100 Mb of memory. If you had 128 Mb of physical RAM, this would leave 28 Mb for Windows and other programs that may be running at the same time as FEMAP.
Licensing Conversion Methods Please read this section very carefully before changing your licensing method. If you are going to convert your licensing method you MUST HAVE FEMAP AND NX NASTRAN CLOSED (not running) before you use the files described below. You can change your licensing method (i.e., from using a security key to using a network license) using specific “batch” files located in the FEMAP directory. The files are named “go_licensing method”.bat and require minimum user input to change your licensing method. In general, the “go” batch files change your current “auth_92.dll” to use the appropriate licensing method (auth_licensing method.dll) and may create or alter some other required files. FEMAP will open a “command prompt” and let you know if the conversion of the auth_92.dll has been successful. The various “go” files are explained in greater detail below: •
go_apionly.bat - converts your current licensing method to the “API Only” version of FEMAP
•
go_demo.bat - converts your current licensing method to the FEMAP 300-Node Demonstration version.
•
go_dongle.bat - converts your current licensing method to use a security key.
•
go_network.bat - converts your current licensing method to use the FlexLM Network Client.
3.
Analyzing Buckling for a Bracket
In this first example, you will explore the buckling load of a simple bracket subject to a concentrated cantilevered load. The bracket, although solid, will be idealized as a thin shell finite element model, fixed at the base and loaded at the tip.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the bracket
•
meshing the model
•
applying constraints and loads
•
analyzing the model using the NX Nastran solver
•
post-processing the results
Importing the Geometry What Import a FEMAP neutral file containing the geometry of the bracket.
How Step
UI
Command/Display
1.
File, New Menu
2.
File, Import, FEMAP Neutral Menu
3-2 Step
UI
Analyzing Buckling for a Bracket
Command/Display
3.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory in your FEMAP installation.
4.
File name: Bracket.NEU Open Neutral File Read Options dialog box: OK
V1
ZX Y
Meshing the Model The first step for the meshing process will be to define the property and material for the elements. Next, you will mesh the surfaces.
Defining the Property and Material The shell property represents the thickness of the material making up the two regions of the part.
What Define the shell element property.
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Elem/Prop Type
3.
Element/Property Type dialog box: Plane Elements: Plate OK
Meshing the Model
Step 4.
UI
3-3
Command/Display Define Property dialog box: Title: Shell Notice: Titles can be up to 79 characters long in FEMAP 9.3 and above
5.
Property Values: Thicknesses: 0.1
6.
OK Yes (to create material) Notice: You have created the property, but you also need to define the associated material. In steps below, you will choose a standard material from the FEMAP material library.
7.
Define Material - ISOTROPIC dialog box: Load
8.
Select from Library dialog box: AISI 4340 Steel (select)
9.
OK, then... In Define Material - ISOTROPIC dialog box: OK, then... In Define Property dialog box: OK Cancel Tip: Once you defined the first property, FEMAP automatically prompted you to enter another property. To end the command, press Cancel. Generally, you will need to press Cancel to exit from any entity creation command.
Meshing the Model The geometry that you imported is simply a wireframe representation of the part’s midsurfaces. To create finite elements in FEMAP, you need to specify the regions, or “boundaries” where you need to mesh. You also need to specify how many elements that you want along the edges of a region. By default, all geometry is assigned a mesh spacing of 1.0. If you mesh this part without specifying a tighter mesh size, your mesh will be too coarse to give meaningful answers. By default, you have been viewing the model in the regular wireframe mode. Once you have created the mesh, you will change to the Free Edge model style to ensure that the part is meshed continuously. Since it isn’t, you’ll use the Coincident Nodes check to merge duplicate nodes at the split between the two regions.
What Create boundary surfaces for both regions of the model.
3-4
Analyzing Buckling for a Bracket
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select the four curves that make up one of the regions (see figure below). OK
3.
Select the four curves that make up the part’s other region. OK Cancel (to end the command)
Notice: You should now have two new boundary surfaces.
V1
ZX Y What Specify the mesh size for the surfaces.
Meshing the Model
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
2.
Entity Selection dialog box: Select All OK
3.
Automatic Mesh Sizing dialog box: Element Size: 0.3 OK Cancel
What Mesh the surfaces.
How Step
UI
Command/Display
1.
Mesh, Geometry, Surface Menu
2.
Entity Selection dialog box: ID: 1 OK
3.
Automesh Surfaces dialog box: Property: Shell OK
4.
Mesh, Geometry, Surface Menu
5.
Entity Selection dialog box: ID: 2 OK
3-5
3-6 Step
UI
6.
Analyzing Buckling for a Bracket
Command/Display Automesh Surfaces dialog box: OK
ZX Y What Display the model using the Free Edge style.
How Step
UI
Command/Display
1.
F5 key
View Select Tip: You can also press the View Select icon (on the toolbar) or View, Select command to open the dialog box.
2.
View Select dialog box: Model Style: Free Edge OK
V1
ZX Y Notice: The model is displayed with only the free edges showing. As expected, there are free edges around the outside of the part. There are also free edges where the part needs to be connected, at the split line between the two regions. This indicates that there are duplicate nodes at these locations, each connected to shell elements on one side of the edge. Tip: If you had selected all the surfaces and meshed them together, the meshes on the two surfaces would have been connected.
Meshing the Model
3-7
What Check for coincident nodes, and merge them.
How Step
UI
Command/Display
1.
Tools, Check, Coincident Nodes Menu
2.
Entity Selection dialog box: Select All OK
3.
Check/Merge Coincident dialog box: Options: Merge Coincident Entities OK Notice: You will notice on the Check/Merge Coincident dialog box that a “Preview Coincident” option exists. When this option is checked, FEMAP will enter a mode which allows you to highlight the nodes which will be “Kept”, “Merged”, or “Both” in your model. Clicking “Done” will complete the operation with the selected options (i.e., listing the coincident nodes to the Messages pane, Merging the nodes, creating the appropriate groups)
4.
Window, Regenerate Menu
V1
ZX Y 5. 6.
F5 key
View Select View Select dialog box: Model Style: Draw Model OK
3-8 Step
Analyzing Buckling for a Bracket
UI
Command/Display
V1
ZX Y
Applying Constraints and Loads Next, you will apply constraints and loads to the model. Since most parts and systems of parts can be held and loaded in any number of ways, FEMAP uses sets to manage constraints and loads. First, you will create a constraint set, then you will fix all of the nodes at the base of the model. Next, you will create a load set, then apply a 100 pound load to the tip of the bracket. In a buckling analysis, the actual loading of the part is applied, and the solver returns a buckling eigenvalue. The eigenvalue is multiplied by the applied load to give the critical buckling load.
Applying Constraints What Create the constraint set.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
What Create the constraints to fix the nodes at the base of the model.
Applying Constraints
How Step
UI
Command/Display
1.
Model, Constraint, Nodal Menu
2.
Entity Selection dialog box: Pick the nodes at the edge of the model. OK
3.
Create Nodal Constraints/DOF dialog box: Fixed OK Cancel
V1 C1
ZX Y 4. 5.
Ctrl-Q keys
123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456
View Quick Options View Quick Options dialog box: Labels Off Done
3-9
3-10 Step
Analyzing Buckling for a Bracket
UI
Command/Display
V1 C1
ZX Y
Applying Loads Apply the 100-pound load to the model.
What Create the load set.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Title: (enter a title) OK
What Create the load in the negative Y direction.
How Step
UI
Command/Display
1.
Model, Load, Nodal Menu
2.
Entity Selection dialog box: Pick node at the tip of arrow (see following figure). OK
Analyzing the Model
Step
UI
3-11
Command/Display
V1 C1
A
ZX Y 3.
Create Loads on Nodes dialog box: FY: Value: 100 Notice: The default load type is force.
4.
Click OK, then... Click Cancel
V1 L1 C1
ZX Y
Analyzing the Model The FEMAP analysis manager stores the options for creating an input file for a solver (an analysis set). It can launch the NX NASTRAN solver or another solver that has been set up to run on the same PC. The analysis manager, together with VisQ, can also set up and run analyses with solvers on other PCs. The analysis sets are stored with the FEMAP model file, and can also be stored in a FEMAP library that can be accessed from different model files.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
3-12 Step
UI
Analyzing Buckling for a Bracket
Command/Display
2.
Analysis Set Manager dialog box: New
3.
Analysis Set dialog box: Title: Buckling
4.
Analysis Program: 36..NX Nastran Analysis Type: 7..Buckling
5.
Click OK
Notice: The analysis set manager displays all analysis sets defined in the model, and the sections that make up the input file for the solver. Clicking on a plus sign will expand the tree and display individual options that can be edited by double-clicking on an option. For this analysis, you’ll use the default values for these options. 6.
Analyze
Notice: The Graphics window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results For this example, you will display the buckling shape and buckling factor.
What Display the deformed model (buckled shape) and the critical buckling factor.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: Deform
3.
Deformed and Contour Data
Post-processing the Results
Step 4.
UI
3-13
Command/Display Select PostProcessing Data dialog box: Output Set: 2..Eigenvalue 1 33.02924 OK (all dialog boxes)
Notice: The set value is the eigenvalue and critical buckling factor for a buckling analysis. In this case, the part would buckle at a load 33.03 times higher than the applied load. This is the end of the example. You don’t need to save the model file.
3-14
Analyzing Buckling for a Bracket
4.
Creating and Meshing a Solid Model In this example, you will use the FEMAP geometry modeling capabilities to build a solid model of a slotted guide. You’ll apply constraints and loads, then mesh the model.
1
To perform this example, you’ll need to have the Parasolid modeling engine active. If you have the 300-node version of FEMAP, you won’t be able to save your model file or change the model after meshing due to size limitations. Y Z
X
The example includes the following steps: •
importing the geometry
•
creating the solid part
•
creating the slot
•
creating the bolt holes
•
creating the guide boss
•
applying constraints and loads
•
meshing the model
Importing the Geometry What Open a new model file and import the FEMAP neutral file containing the basic profile for the part.
How Step
UI
Command/Display
1.
File, New Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory.
4-2 Step
UI
Creating and Meshing a Solid Model
Command/Display
4.
File name: Slot.NEU Open
5.
Neutral File Read Options dialog box: OK Notice: The imported curves will form the base of the part.
V1
Y ZX
Creating the Solid Part To create the part, you’ll first create a boundary, then extrude it.
What Create a boundary from the curves.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select All OK Cancel
What Extrude the boundary to form a solid part.
Creating the Solid Part
4-3
How Step
UI
Command/Display
1.
Geometry, Solid, Extrude Menu
Notice: Since there is only one boundary, the software selects it automatically. 2.
Material: New Solid Direction: Negative Length: To Depth
3.
To Depth: 10 OK
4.
Dynamic Rotate (on View Toolbar)
5.
Dynamic Display dialog box: Hold the left mouse button and rotate the model to see the extrusion. OK Tip: If you are in Render mode, you do not have to pick the Dynamic Rotate icon on the toolbar before using the mouse to dynamically rotate your model. Render mode is the default graphics mode and uses the OpenGL graphics language. Render mode can only be turned off by using the View, Options command. Once the View Options dialog box is open, select Tools and View Style in the Category section, then select Render Options from the list of Options. Click the Graphics Engine button and select Windows GDI in the dialog box, then Click OK and OK again. There is NO reason to turn off Render mode when doing the Examples.
6.
Click OK when you are done rotating the model.:
V1
Y Z X
4-4
Creating and Meshing a Solid Model
Creating the Slot What To start drawing the slot, create two circles.
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
2.
Locate dialog box: 0, 95, 0 (enter these X, Y, Z values for the center of the circle) OK
3.
11, 95, 0 (enter a point on the circle) OK Notice: FEMAP prompts you to create another circle.
4.
Define another circle: 0, 50, 0 (center), Click OK, then... 11, 50, 0 (point on the circle), Click OK, then Cancel
V1
Y ZX What Finish creating the geometry of the slot.
Creating the Slot
4-5
How Step
UI
Command/Display
1.
Geometry, Curve - Line, Points Menu
2.
Create Line from Points dialog box: Pick points A and B. OK
V1 C
A A
D
B
Y ZX 3.
Create another line from points C to D. Click OK, then Cancel
V1
Y ZX What Break the circles into 2 parts.
How Step 1.
UI
Command/Display Snap to Point can be found on Select Toolbar snap modes menu or from on the Quick Access Menu (click right mouse button in graphics window) Tip: The snap modes can also be chosen using the “Right Mouse Menu” in FEMAP. Simply right-click the mouse in the graphics window and choose the appropriate snap option.
4-6 Step
UI
Creating and Meshing a Solid Model
Command/Display
2.
Modify, Break Menu
3.
Entity Selection dialog box: Pick the lower circle. OK
4.
Locate dialog box: Pick point A (in following figure). OK Tip: You need to check that the view axes are oriented the same as in the following figure. If the model is reversed and you pick the points opposite A and B, you will be picking the end point of the circular curves and the split will fail.
V1 B
A
Y ZX 5.
Pick the upper circle, then break it at point B.
6.
Delete, Geometry, Curve Menu
7.
Entity Selection dialog box: Pick the two inner halves of the circles.
Creating the Slot
Step
UI
4-7
Command/Display
8.
OK Yes (delete the curves) Tip: The Update Views check box on the Confirm Delete dialog enables you to automatically regenerate the graphics after the deletion. If you are doing a lot of deletes in a large model, you might want to uncheck this box to improve performance and then press Ctrl-G to regenerate the display when you have finished deleting entities
V1
Y ZX What Create a boundary surface and extrude the new curves.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Pick the four curves of the slot. OK, then... Cancel
4-8 Step
UI
Creating and Meshing a Solid Model
Command/Display
3.
Geometry, Solid, Extrude Menu
Notice: The boundary that you just created is already selected. 4.
Extrusion Options dialog box: Material: Remove - Hole Direction: Negative Length: Thru All OK
V1
Y Z X
Creating the Bolt Holes You’ll now use a patterning technique to create five bolt holes.
What Use a pattern to create five bolt holes.
Creating the Bolt Holes
4-9
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
-38, 0, 0 (center), Click OK, then... -38, 5, 0 (a point on the circle), Click OK, then... Cancel
V1
Y ZX 2.
Geometry, Boundary Surface, From Curves Menu
Pick the circle. OK, then Cancel 3.
Geometry, Solid, Extrude Menu
4.
Extrusion Options dialog box: Material: Remove Hole Direction: Negative Length: Thru All Tip: Make sure that the Extrude arrow extends through the thickness of the part. If it points the wrong way, change the Direction.
5.
Pattern
6.
Patterns dialog box: Radial
7.
Center: 0, 0 (XY coordinates) Number: 5 Total Angle: 180 OK (all dialog boxes)
4-10 Step
UI
Creating and Meshing a Solid Model
Command/Display
V1
Y ZX
Creating the Guide Boss Next, create the guide boss and its slot.
Creating the Guide Boss What Create the geometry of the guide boss.
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
2.
For the first circle, enter: 0, 0, 0 (center) 25, 0, 0 (point on circle)
3.
For the second circle, enter: 0, 0, 0 (center) 16, 0, 0 (point on circle)
4.
Zoom (on View Toolbar) Pick two corners to draw a box around the two new circles.
Creating the Guide Boss
Step
UI
4-11
Command/Display
V1
Y ZX 5.
Geometry, Boundary Surface, From Curves Menu
Select the two new curves. OK 6.
Geometry, Solid, Extrude Menu
7.
Extrusion Options dialog box: Material: Add - Protrusion Direction: Positive Length: To Depth
8.
To Depth: 50 OK Tip: To better see the model, rotate it and change to a solid model display: pick the View Style icon on the View Toolbar, then pick Solid. To restore the display, pick View Style, then pick Wireframe.
4-12
Creating and Meshing a Solid Model
Creating the Guide Boss Slot Create the slot in the guide boss.
What Move the workplane to the top of the boss, so that you can more easily build the slot. The workplane is a two-dimensional plane that you can locate and align anywhere in three-dimensional space. When you make a graphical selection, the screen location that you selected is projected along a vector normal to the screen onto the workplane. The resulting three-dimensional coordinates are located at the intersection of the projection vector and the workplane. How Step
UI
Command/Display
1.
Tools, Workplane Menu
2.
Draw Workplane (check)
3.
On Surface
4.
Plane Normal to Surface dialog box: On Surface: (pick the surface highlighted below) At Point: (pick point A) Axis Point: (pick point B) OK
A
B
What Create the boss slot. First, you’ll create a horizontal line on the surface of the boss. Next, you’ll create two parallel lines, and use them to form a rectangle. Finally, you’ll extrude the rectangle to create the slot.
Creating the Guide Boss Slot How Step
UI
Command/Display
1.
Geometry, Curve - Line, Points Menu
2.
Create Line from Points dialog box: From Point: (pick point A from previous diagram) To Point: (pick point B) OK Notice: There is a new horizontal line on the surface of the guide boss.
V1
Y ZX 3.
Geometry, Curve - Line, Parallel Menu
4.
Line Parallel to a Line dialog box: From Curve: (pick the curve you just created) Offset: 3.5 OK
5.
Locate dialog box: Pick a point to one side of the line, such as point A below. OK
4-13
4-14 Step
UI
Creating and Meshing a Solid Model
Command/Display B
V1
Y ZX 6.
A
Pick the line again. Pick a point on the other side of the line, such as point B above.
Notice: The guide boss now has three parallel lines on the top.
V1
Y ZX 7.
Geometry, Curve - Line, Points Menu
8.
Create Line from Points dialog box: From Point: Pick point A (the endpoint of the top line) in the following diagram. To Point: Pick point B. OK
V1
A
C
B
D
Y ZX
Creating the Guide Boss Slot
Step
UI
Command/Display
9.
Create another line between points C and D.
10.
Geometry, Boundary Surface, From Curves Menu
11.
Pick the four curves below to form a rectangle.
V1
Y ZX 12.
Geometry, Solid, Extrude Menu
13.
Extrusion Options dialog box: Material: Remove - Hole Direction: Negative Length: To Depth
14.
To Depth: 12 OK
4-15
4-16
Creating and Meshing a Solid Model
Applying Constraints and Loads For constraints, fix the bolt holes. Next, create a load on the inner surface of the slot.
What Create a constraint set, then apply constraints to the bolt holes.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
3.
Model, Constraint, On Surface Menu
4.
Entity Selection dialog box: Pick the 10 inner surfaces of the bolt holes. OK
5.
Create Constraints on Geometry dialog box: Fixed OK
Applying Constraints and Loads
Step
UI
Command/Display
V1 C1
Y ZX 6.
Ctrl-A
Autoscale the model (display the entire model in the Graphics window).
V1 C1
Y Z X What Create the load set, then apply a load of -1000 pounds to one face of the slot.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Title: (enter a title) OK
3.
Model, Load, On Surface Menu
4-17
4-18 Step 4.
UI
Creating and Meshing a Solid Model
Command/Display Entity Selection dialog box: Pick one face inside the slot (see the following figure). OK
Tip: Rotate and zoom the model so that you can more easily see the face. 5.
Create Loads on Surfaces dialog box: FX: Value: -1000 OK
V1 L1 C1
Y ZX
Meshing the Model Define the property and material for the model, then generate a solid mesh.
Defining the Property and Material What Define the solid element property.
Defining the Property and Material
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Elem/Prop Type
3.
Element Property Type dialog box: Volume Elements: Solid OK
4.
Title: Solid OK Notice: Titles can be up to 79 characters long in FEMAP 9.3 and above
5.
Yes (to create material)
6.
Define Material - ISOTROPIC dialog box: Load
7.
Select from Library dialog box: AISI 4340 Steel (select)
8.
OK (all dialog boxes), then... In Element Property Type dialog box: Click Cancel
What Create a solid mesh for the model.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Automesh Solids dialog box: OK
4-19
4-20 Step
UI
Creating and Meshing a Solid Model
Command/Display
V1 L1 C1
Y Z X This is the end of the example. You don’t need to save this model file.
5.
Working with Groups and Layers
The FEMAP group and layer capabilities enable you to segment your model into smaller, more manageable, discrete pieces. You can then use these pieces to minimize the amount of information displayed in the Graphics window or included in a printed report. Groups and layers also make it easier to manipulate, update, and apply loads to your model. This example introduces groups and layers. •
FEMAP groups identify portions of your model. Once you create a group, you can limit your display to the portion of the model that is in the group. In addition, a group can impact post-processing. For instance, FEMAP can automatically adjust contour/criteria limits to the peak values that occur on the entities in the group. You can also easily group elements using a particular property or material.
•
FEMAP layering is similar to layering in most CAD systems. In FEMAP, you can think of a layer as a clear sheet of “paper” with entities drawn on it. The display of the model may include many layers overlaid on one another. You can control which entities are displayed by defining which layers are visible.
Other FEMAP capabilities that control how the display of your model include the View - Select and View - Options menus, as well as post-processing displays. These features are explored in other examples.
Differences Between Groups and Layers Both groups and layers enable you to control the display of your model. However, there are some key differences between groups and layers:
Groups
Layers
An entity can be included in multiple groups.
An entity can be included in only one layer.
Only one group can be displayed at a time.
Multiple layers can be displayed at the same time.
Only one group can be active. (You can only work with one group at a time.)
Only one layer can be active. (You can only work with one layer at a time.)
See Also •
Section 5.9.2, "Groups and Layers Overview" in the FEMAP User Guide
•
Section 6.4, "Groups and Layers" in FEMAP Commands
Using Groups In this series of examples, you’ll use the wing model to create and work with several different groups.
Creating a Group What Open the model file containing the wing model. Change the view style to quick hidden line, and turn off the display of loads and constraints.
5-2
Working with Groups and Layers
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Wing.MOD file.
V1 L1 C1
Y Z X 3.
File, Save As Menu
Save the model file with a different name. 4.
View Select (on View Toolbar)
5.
View Select dialog box: Model Style: Quick Hidden Line OK
6.
Quick Options (on View Toolbar)
7.
View Quick Options dialog box: Load/Constraint Off Done
Creating a Group
Step
UI
5-3
Command/Display
V1 L1 C1
Y Z X What Create a group that represents just the upper and lower wing skins.
How Step
UI
Command/Display
1.
Group, Set Menu
Tip: You can also create a new Group using the New command on the “context sensitive menu” located on the Groups branch in the Model Info tree (simply click to highlight the top level of the Groups branch or any existing Group, then right mouse click to see the context sensitive menu). 2.
Create or Activate Group dialog box: Title: Wing Skins OK
3.
Group, Element, Property Menu
4.
Entity Selection dialog box: Pick one plate element from the top wing skin (property 101). Pick one plate element from the bottom wing skin (property 102). Rotate the model if necessary. OK Notice: As you select elements on the screen, FEMAP extracts the element’s property and fills the selection box accordingly.
What Display the new group.
5-4
Working with Groups and Layers
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Group: Select Tip: For a shortcut to the Model Data command, right-click in the Graphics window. From the menu, pick Model Data.
4.
Wing Skins (pull down menu and pick) OK (all dialog boxes)
Using a Group to Trim a Report In this next section of the example, you’ll see how groups can be useful in creating a report. Perhaps you are interested in finding the element in either the upper or lower wing skin with the maximum shear flow (FXY force). You’ll use the wing skin group to find this element.
What Create the report based on the wing skin group.
How Step
UI
Command/Display
1.
List, Output, Standard Menu
Using a Group to Trim a Report
Step
UI
5-5
Command/Display
2.
Entity Selection dialog box: OK
3.
List Formatted Output dialog box: Title: Maximum Shear Flow
4.
Sort Field: 7208: Plate XY Membrane Force
5.
Top N: Top
6.
Number: 5
7.
Format ID: 8..NASTRAN QUAD4 Forces
8.
Options: Details Only OK
9.
Entity Selection dialog box: Group: Wing Skins OK Notice: The report appears in the Messages dockable pane.
10.
Ctrl - U
Notice: Ctrl-U undocks the Messages dockable pane. The report lists the plate element forces corresponding to the top five shear flow plates in the upper and lower wing skins. The report is sorted in ascending order. You can now easily see that the maximum shear flow (FXY) is 62.31 lb./inch, and is in element 120.
11.
Ctrl - U
(Toggle back to the regular view style.)
What Quickly find element 120.
How Step
UI
Command/Display
1.
Window, Show Entities Menu
5-6 Step
UI
Working with Groups and Layers
Command/Display
2.
Entity Show dialog box: Entity Type: Element OK
3.
Entity Selection dialog box: ID: 120 OK Notice: Element 120 is temporarily highlighted.
Tip: As you’ve just seen, a group can be used in the standard entity selection box. Any time FEMAP prompts you to select entities, you can specify a group. This feature can be extremely useful when you are applying loads to a portion of your model, or when you want to update sections of your model.
Automatically Generating Groups Once you become proficient in FEMAP, you’ll probably find yourself creating groups as you build a finite element model to keep important areas of the model together for use downstream. If you don’t do this, or if you import an existing model, FEMAP has several tools for automatically grouping together portions of your model based on changes in material properties, element properties, or even geometric regions. This example shows you how to automatically split the wing mode into groups based on properties.
What Automatically generate groups based on properties.
How Step
UI
Command/Display
1.
Group, Operations, Generate Property Menu
2.
Entity Selection dialog box: Select All OK
Using the Group Information
Step
UI
5-7
Command/Display Notice: You’ve just created groups of elements based on the nine different properties in this model.
3.
Model Data
4.
Group: 2..Property 1: Upper Angle Stiffener OK Notice: The stiffeners group is displayed. If you would like “toggle on” the cross-sections of line elements and/or the thickness of plate elements for viewing, select Thickness/Cross Section from the View Style menu located on the View Toolbar
5.
Use the Model Data dialog box to display each of the other groups. Tip: You can use the Model Info tree to quickly switch the group currently being viewed. Simply expand the Groups branch so all the groups in the model are visible in a list. Highlight any group in the list and then click the right mouse button to access the “context sensitive menu” for Groups. Selecting View Active from the menu will change the view so only the “Active” group is visible. You can change the “Active” group by double-clicking on any other group in the list (the title of the group will go from black to blue text to signify the group is now “Active”). Set Model Data to Group:None in this model to use this method. Tip: You can “combine” groups very easily using the Model Info tree. Select any number of groups using the Ctrl or Shift keys and the mouse. Once the groups are selected, right mouse click and choose the Combine command. This will place all of the entities of the selected groups into one new group which can then be made “Active” to be viewed. Tip: Other than Combine, there are 5 other “boolean operations” which can be used to create new groups from multiple groups via the Group, Operation, Boolean command.
Using the Group Information In this section of the example, you’ll use a group to display specific information about the model.
What Display the axial forces in the upper stringers.
5-8
Working with Groups and Layers
How Step
UI
Command/Display
1.
Model Data
2.
Group: 6..Property 5 - Upper Stringer - T Section OK
3.
View Select (on View Toolbar)
4.
View Select dialog box: Contour Style: Criteria
5.
Deformed and Contour Data
6.
Select PostProcessing Data dialog box: Output Vectors: Contour: 3022..Beam EndA Axial Force OK (all dialog boxes) Notice: FEMAP now displays a criteria plot of the axial forces for the elements displayed.
Using Layers
5-9
Using Layers Working with layers is quite easy as long as you understand the basic layering concepts: every entity in FEMAP references a layer, and a layer is either on or off. The View, Layers command controls which layers are displayed. This section of the example shows you how to work with layers.
What Reset the display of the wing model.
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Contour Style: None
3.
Model Data
4.
Group: None OK (all dialog boxes)
V1 L1 C1
Y Z X What View the different layers in the model.
How Step
UI
Command/Display
1.
View, Layers Menu
Tip: You can also pick the Layers icon on the toolbar.
5-10 Step 2.
UI
Working with Groups and Layers
Command/Display Layer Management dialog box: Show Visible Layers Only
3.
Hidden Layers: 2..Middle Section
4.
Show
5.
Visible Layers: 1..Inner Section
6.
Hide
7.
Hide the Outer Section layer. OK
V1 L1 C1
Y Z X 8.
Layers (on View Toolbar)
9.
Layer Management dialog box: Make the following layers Hidden: Construction Layer, 2..Middle Section. Make the following layers Visible: 1..Inner Section, 3..Outer Section. OK Tip: You can “hide and show” layers very easily using the Model Info tree. Select any number of layers using the Ctrl or Shift keys and the mouse. Once the layers are selected, right mouse click and choose the Make Visible or Make Hidden commands. You can also choose to Show All Layers or Show Visible Layers Only by selecting those commands from the “context sensitive menu” for Layers
Using a Contour Group for Post-processing
Step
UI
5-11
Command/Display
V1 L1 C1
Y Z X 10.
Layers (on View Toolbar)
11.
Layer Management dialog box: Show All Layers OK
V1 L1 C1
Y Z X
Using a Contour Group for Post-processing Sometimes you may want to create an image that displays the results on a single group of elements while showing the rest of the model as a “reference”. This can be accomplished by setting a “Contour Group” in the Contour Options dialog box.
What Choose a “contour group” in the contour options dialog box.
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Contour Style: Contour
5-12 Step
UI
Working with Groups and Layers
Command/Display
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Contour: 7033..Plate Top VonMises Stress
5.
Contour Options
6.
Select Contour Options dialog box: Contour Group: Select
7.
Group: 7..Property 101 - Upper Wing Skin
8.
OK (all dialog boxes)
This is the end of the example. You don’t need to save the model file.
6.
Working with View Select and View Options
FEMAP provides a wide variety of viewing options that help you be more productive. This example introduces two dialog boxes that control how your model is displayed on the screen: View Select and View Options. •
View Select controls the top level display options. With View Select, you can control whether your model is displayed in hidden line or plain wireframe mode, turn on and off stress contours, animations, deformed plots, etc.
•
View Options provides the detailed control over how entities are displayed: element color, node label display, perspective, etc. View Options also provides extensive control over post-processing options.
Other FEMAP capabilities that control how the display of your model include groups, layers, and post-processing displays. These features are explored in other examples.
Using View Select The View Select dialog box lets you control the following types of view information: •
XY Style: Controls XY plot appearance.
•
Model Style: Controls general model display.
•
Deformed Style: Controls display of deformed plots for post-processing.
•
Contour Style: Controls display of contour plots for post-processing.
The following example lets you explore some of the Model Style options. You will explore the other types of view information in the post-processing examples. For more information on View Select, see: •
Section 5.9, "Groups, Layers and Viewing Your Model" in the FEMAP User Guide
•
Section 6.1.5, "View, Select and View, Options" in FEMAP Commands
•
Section 8.2, "Types of Views - View Select..." in FEMAP Commands
What Open the model file containing the wing model.
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory.
6-2 Step
UI
Working with View Select and View Options
Command/Display Filename: Wingpost.MOD Open
V1 L1 C1
Y Z X 3.
Save the model file with a different name. Tip: Use File, Save As.
What Explore Hidden Line options.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Full Hidden Line OK Notice: Full Hidden Line shows only the entities that are visible. In Render mode, Full Hidden Line and Quick Hidden Line are the same. In non Render mode, Full Hidden Line is more accurate than Quick Hidden Line, but is slower to display.
V1 L1 C1
Y Z X
Using View Options
6-3
What On the View Select dialog box, you can use the Model Data button to control the display of load sets, constraint sets, groups, and functions. In this example, you’ll display the second load set in the model.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Load Set: Select
4.
Pressure Distribution OK (all dialog boxes) Notice: The pressure load set is now visible. Rotate the model for a better view.
C1
Y Z X 5.
View Select (On View Toolbar) dialog box: Under Model Data, select the Wingtip Loading load set. Don’t close the model file yet. You will use it in the next part of the example.
Using View Options The View Options dialog box lets you control the following categories of view information: •
Labels, Entities, and Color: Controls the display of model entities, such as nodes and elements. You can choose whether entities will be drawn, if and how they will be labeled, and the colors that will be used.
•
Tools and View Style: Controls display of tools, such as the workplane. This category also lets you control the style of the settings for free edge, element filling, shading, and perspective options. Additional options let you control view-related items such as the legend, origin, and view axes.
•
Post Processing: Controls all of the graphical post-processing options, including deformed, contour, criteria, and XY plots. None of these options, however, will have any effect unless you select one of the post-processing options through View Select.
In this example, you’ll explore the first two categories on the View Options dialog box. For more information on View Options, see:
6-4
Working with View Select and View Options
•
Section 6.1.3, “View Select and Options” in FEMAP Commands
•
Section 8.3, “View Options: Postprocessing” in FEMAP Commands
What Display the elements based on their property color.
How Step
UI
Command/Display
1.
View, Options Menu
2.
View Options dialog box: Labels, Entities, and Color (select)
3.
Options: Element (select)
Notice: The options on the right side of the dialog box change. 4.
Color Mode: 3..Property Colors (select) Apply (don’t press OK)
Notice: Press Apply to see the effects of the change without exiting the dialog box. Initially, elements are displayed based on their own (entity) color. When you change the display to Property Colors, FEMAP displays each element using the element property’s color. This capability is very useful for visualizing how the various properties in your model are distributed, and to help you ensure that elements reference the appropriate properties. 5.
You can rotate the model using the mouse while pressing the middle mouse button. If you do not have a three button mouse, press the Dynamic Rotate icon in the toolbar.
Using View Options
6-5
What Shrink the elements to make the borders of the properties easier to see.
How Step
UI
Command/Display
1.
Category: Tools and View Style
2.
Options: Shrink Elements
3.
Option On (check) Apply
Tip: In the Options list, you can double-click on the option name to toggle it on and off.
What Display the elements filled in.
How Step
UI
Command/Display
1.
Options: Fill, Backspace, and Hidden
2.
Fill On (check) OK Notice: The model is now displayed with the elements filled with their property colors.
6-6 Step
UI
Working with View Select and View Options
Command/Display
Notice: All of the options explained in the Using View Options section of this example (and more) are also available from the View Style menu located on the View Toolbar:
For instance, to quickly change the Color Mode from “Entity” to “Property” Color, choose the Color With... (Entity Colors/Property Colors/Material Colors) command on the View Style menu. In addition, the Fill and Shrink commands on the View Style menu will perform the same operations used in this example. This is the end of the example. You don’t need to save the model file.
7.
Using Post-Processing
Once you have obtained results from an analysis, you can view these results either graphically or as reports. FEMAP graphical post-processing includes deformation plots, contour/criteria plots, XY plots, and freebody plots. The graphical results can be displayed on the screen or output as a file. Report-based post-processing provides text output of post-processing data with a variety of formats, printing options, and sorting options. In this set of examples, you will explore the following FEMAP graphical post-processing capabilities: •
Deformation and contour results: You will select contour options as well as display dynamic isosurfaces and cutting planes.
•
XY plots: You will generate an XY plot of results and also generate a new results vector.
•
Results displays in other applications. You will use a deformation/contour plot in a word processing application, and an animation in a presentation application.
For more information on post-processing, see: •
Section 5, "The FEA Process" in the FEMAP User Guide
•
Section 8, "Post-Processing" in FEMAP Commands
Post Processing Overview The basic FEMAP post-processing procedure is as follows: 1. Obtain analysis results. FEMAP automatically recovers the results from many analysis programs. If your analysis program doesn’t allow this automatic recovery, you can import results (File, Import, Analysis Results). Note that analysis output data is stored in sets. If you run your model with several different loading conditions or analysis types, FEMAP will keep the output data from each analysis, mode shape, or time step in a different output set. 2. Define the type of plot and the data to be displayed. From the View Select dialog box, you can choose the type of XY, deformed, or contour plot to display. You can also select the data to be displayed. 3. Define detailed display options. From the View Options dialog box, you can control options that include the appearance of titles, deformed/undeformed model display, number of levels in a contour plot, etc.
Generating Deformation and Contour Results You can display results as deformations, contours, or combine both types of plots in the same view. From the View Select dialog box, you can select the following types of deformed and contour data: Plot Type
Description
Deformed Style: Deform
A plot of the deformed shape.
Animate
An animation of the deformed shape.
Animate MultiSet
Animation across several output sets. Good for transient, nonlinear, and frequency response analysis.
Vector
A plot showing vectors representing direction and magnitude of output.
7-2
Using Post-Processing
Plot Type
Description
Trace
Displays trace lines connecting historical positions of nodes.
Contour Style: Contour
Displays contour areas or lines.
Criteria
Displays elemental values at the centroids of elements.
Beam Diagram
Displays results along the length of line elements. Similar to 3D shear and bending moment diagrams.
IsoSurface
Displays interior surfaces of constant values in solid models.
Section Cut
Shows contours through any planar cut of a solid model.
Vector
Displays vectors at the centroids of elements.
Note: For multi-set animation and trace plots, you can also choose to animate only the contours. These types of plots can be extremely useful for heat transfer analyses.
Example A: Generating a Deformed and Contour Plot In this section of the example, you will generate a deformed and contour display.
What Open the model file containing a fan blade model and results from a linear statics analysis.
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Fanpost.MOD file.
3.
Save the model file with a different name.
Example A: Generating a Deformed and Contour Plot
7-3
What Select the deformed and contoured plot types, and specify the post-processing data for the results. Finally, you’ll specify the method used to contour the results.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Deformation: Total Translation Output Vectors: Contour: Solid VonMises Stress
5.
Contour Options
6.
Select Contour Options dialog box: Data Conversion: Max Value
7.
OK (all dialog boxes)
Notice: The data conversion options control how FEMAP converts the results from pure data at element centroids, corners, and nodes to the continuous graphical representation. In this example, you’ve chosen the maximum value using corner data. To calculate the value of an interior node in this mesh, the software takes the maximum value of the data at the corners.
7-4
Using Post-Processing
What Generate another deformed/contour plot using the averaged data conversion option.
How Step
UI
Display/Command
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Contour Options
4.
Select Contour Options dialog box: Data Conversion: Average
5.
OK (all dialog boxes)
Notice: You’ve now chosen the average value using corner data. To calculate the value of an interior node in this mesh, the software takes the average value of the data at the corners. Tip: You can use the difference in the maximum and average results to make a quick estimate of the fidelity of the model. If there is a large difference between these two contours, especially at locations that don’t have sharp corners or breaks in the model, then your model may require a finer mesh. 6.
Don’t close the model file. You will need it for Example B.
Example B: Displaying Dynamic Isosurfaces and Cutting Planes In this example, you’ll display: •
dynamic isosurfaces. You can dynamically change the value of the displayed isosurface.
•
dynamic cutting planes. You can choose an arbitrary cutting plane and dynamically pass it through a solid model.
Example B: Displaying Dynamic Isosurfaces and Cutting Planes
7-5
What Change the appearance of the plot by turning off display of the undeformed model and filled edges.
How Step
UI
1. 2. 3.
Command/Display Use the fan blade model from Example A.
F6 key
View Options View Options dialog box: Category: PostProcessing
4.
Options: Undeformed Model
5.
UNCHECK Draw Entity (turn off)
Notice: The “undeformed” model can be toggled on and off quickly using the Undeformed command from the Post Options menu on the Post Toolbar. 6.
Category: Tools and View Style
7.
Options: Filled Edges
8.
UNCHECK Draw Entity OK Notice: The “element edges” (as well as surface edges) can be toggled on and off quickly using the Filled Edges command from the View Style menu on the View Toolbar
7-6
Using Post-Processing
What View the regions of constant stress.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Display the filled edges again.
3.
View, Advanced Post, Dynamic IsoSurface Menu
4.
Dynamic IsoSurface Control dialog box: Move the slider bar. OK Notice: The display shows regions with the stress value selected on the dialog box.
What Dynamically display a plane cut.
How Step
UI
Command/Display
1.
View, Advanced Post, Dynamic Cutting Plane Menu
Generating XY Plots
Step
UI
2.
7-7
Command/Display Dynamic Section Cut Control dialog box: Move the slider bar.
Notice: The display shows contour values along a plane cut through the model. To change the plane, pick the Plane button.
3.
Save and close this model file. You will need it for Example D.
Generating XY Plots FEMAP can generate XY plots of results. The View Select dialog box also controls whether an XY plot is displayed, and the type of XY plot. The types include: Plot Type
Description
XY vs ID
Plots XY data as a function of ID number for an output vector in one output set.
XY vs Set
Plots XY data versus the output set number for an output vector across several output sets.
XY vs Set Value
Similar to XY vs Set, except that it uses the output set value for X.
XY vs Position
Plots XY data versus the position of nodes or elements along an axis direction for an output vector in one output set.
XY of Function
Plots XY data for functions. Not a post-processing option.
Example C: Generating an XY Plot In this example, you’ll display a plot of VonMises stress, then create and display a new vector of nodal stresses.
What Open the model file containing a plate model and results from a linear statics analysis.
7-8
Using Post-Processing
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Platepost.MOD file.
3.
Save the model file with a different name.
What Generate an XY plot of the plate top VonMises stresses.
How Step
UI
Command/Display
1.
F5 key
View, Select
2.
View Select dialog box: XY Style: XY vs Position
3.
XY Data
4.
Select XY Curve Data dialog box: Output Set: NX NASTRAN Case 1 Output Vector: 7033: Plate Top VonMises Stress OK (all dialog boxes)
Example C: Generating an XY Plot
Step
UI
7-9
Command/Display
5.
Notice: This graph plots all element centroid values vs. position, which is not very useful. You’ll create another vector below.
What Create a new vector of nodal stresses, based on the VonMises stresses.
How Step
UI
Command/Display
1.
Model, Output, Process Menu
2.
Model Output Process dialog box: Options: Convert
3.
Options: Avg
4.
Output Set: 1..NX NASTRAN Case 1
5.
Output Vector: 7033:Plate Top VonMises stress
7-10 Step
UI
Using Post-Processing
Command/Display
6.
Add Operation OK Notice: The dialog box lets you process several output operations at the same time. In this case, the software creates a new vector with nodal data that is based on the vector. The screen display won’t change.
What Make a group of the nodes on the top curve to reduce the amount of data being plotted.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Model Style: Draw Model OK
3.
Group, Set Menu
4.
Create or Activate Group dialog box: Title: Top Nodes OK
5.
Group, Node, On Curve Menu
6.
Entity Selection dialog box: Pick the straight curve on the top edge of the part. OK
Example C: Generating an XY Plot
What Plot the new group with the new nodal output vector.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: XY Style: XY vs Position
3.
XY Data
4.
Select XY Curve Data dialog box: Group: Select
5.
Group: Top Nodes
6.
Output Vector: 300000..Avg Converted Vector 7033 OK (all dialog boxes)
7.
Save the FEMAP model file. You will use it in Example E.
7-11
7-12
Using Post-Processing
Using Results Displays in Other Applications FEMAP provides several ways of using results displays in other applications. You can: •
Copy the active view to the clipboard using File, Picture, Copy. The copied data depends on which FEMAP graphics mode you are using. If you are using Render mode, a bitmap (DIB) is placed on the clipboard and if you are using non Render mode a vector image as well as a bitmap is placed on the clipboard. You can then paste the image into any other Windows program. See Example D.
•
Save the active view as a standard Windows bitmap or a Windows Device Independent Bitmap. To do this, use File, Picture, Save.
•
If the selected view is animating, create movie (AVI) files. You can also use a special bitmap format that can be displayed with the FEMAP replay program, or create a series of bitmaps to be processed by other programs to create animated GIFs for the Internet. See Example E.
•
Write the current model out as a VRML file that can be shared across the network or web with a standard VRML viewer. You can write out solid geometry or meshes.
Example D: Displaying a FEMAP Graphic in Another Application In this example, you will copy graphic displays to Microsoft Word. If you don’t have this program, try using a similar Windows application.
What Copy the deformation/contour displays to a Microsoft Word document. How Step
UI
Command/Display
1.
Open the model file that you saved at the end of Example B.
2.
Display the deformation/contour plot from Example A. Make sure that undeformed geometry is on (View Options), and that data conversion set to Average (View Select, Deformed and Contour Data, Contour Options).
3.
File, Picture, Copy Menu
Notice: This command puts a copy of the plot on the Windows clipboard.
Example D: Displaying a FEMAP Graphic in Another Application
Step 4.
UI
7-13
Command/Display Open Microsoft Word. Pick Edit, Past Special. Paste the graphic as a Device Independent Bitmap.
5.
In the Word document, enter a title for the figure.
6.
Return to FEMAP and change the data conversion option to Max Value. Generate the plot, and copy it into the Microsoft Word document. Enter another figure title.
7-14 Step
UI
7.
Using Post-Processing
Command/Display Close Microsoft Word. Close the FEMAP. You don’t need to save the model file.
Example E: Using an Animation in Another Application In this example, you will animate a deformed/contour display, save it as a movie file, and add it to a presentation created in Microsoft Power Point. (If you don’t have this program, try using a similar Windows application.)
What Animate the model.
How Step
UI
1. 2.
Command/Display Open the model file that you saved in Example C.
F5 key
View Select
3.
Model Data
4.
Select Model Data for View dialog box: Group: None Load Set: None Constraint/DOF Set: None OK
5.
Model Style: Quick Hidden Line Contour Style: Contour
6.
View Select dialog box: Deformed Style: Animate OK
Example E: Using an Animation in Another Application
Step
UI
7-15
Command/Display
Notice: The initial animation is very fast. You’ll need to adjust the speed.
What Adjust the animation speed and refine the display.
How Step
UI
Command/Display
1.
View, Advanced Post, Animation Menu
2.
Animation Control dialog box: Slower (press several times) OK
3.
Post Options (on Post Toolbar) Note: If the Post Toolbar is not showing, use the Tools, Toolbars, Post to make it visible
4.
Undeformed (toggle off)
5.
Post Options (pick the icon again) Scale Deformation
6.
Deformation Scale dialog box: 2 OK
7-16 7.
Using Post-Processing
Post Options (pick the icon) Animation Frames
8.
Animation Frames dialog box: 10 OK
9.
Post Options (icon) Animate: Positive Only (turn on)
10.
Post Options (icon) Animate Contours (turn on)
11. 12.
F6 key
View Options View Options dialog box: Category: Tools and View Style
13.
Filled Edges Draw Entity (turn off)
What Save the animation as a movie file (.AVI), and insert it into a presentation.
Example E: Using an Animation in Another Application
How Step
UI
Command/Display
1.
File, Picture, Save Menu
2.
Save Picture File As dialog box: Files of Type: Video for Windows (*.AVI) Title: Animated Plate Save OK
3.
Open Microsoft Power Point. Open an empty presentation.
4.
Insert, Movies and Sounds, Movie from File Pick the file. Double-click on the image. Notice: The image plays once.
5.
Right-click on the image. Edit Movie Object
6.
Play Object dialog box: Loop Until Stopped Rewind movie when done playing OK Notice: The image plays continuously until you end the program.
7-17
7-18 Step
7.
UI
Using Post-Processing
Command/Display
Close Microsoft Power Point. Close FEMAP. You don’t need to save the model file.
This is the end of the example. You don’t need to save the model file.
8.
Preparing Geometry for Meshing
In this example, you will learn to identify surface shapes that can cause meshing problems, then how to correct the problems to improve the mesh quality. The example includes the following steps: •
understanding the problem
•
preparing the geometry for meshing
•
creating new boundary surfaces
•
suppressing features
•
meshing the model
•
applying loads and constraints
Understanding the Problem V1
In this example, the part is a bearing block used in a large piece of industrial machinery as a simple shim. It is subject to a very large vertical load. You will be examining the amount of vertical deflection due to the vertical load. To generate a good-quality mesh on this part, you will address two issues: • Due to some fine changes in shape, the front and back faces of the part are split into three distinct faces, some of them very poorly shaped for meshing. • The part contains features (the holes) that are not important for the analysis.
ZY X To create a solid mesh, FEMAP first meshes the outside surface of the model with triangles. Every triangle is connected to three others, one on each edge. Then, based on the surface mesh, FEMAP meshes the inside volume with tetrahedral elements.
Preparing the Surfaces for Meshing
V1
If the faces of the solid are poorly shaped or degenerate, the surface mesh may have poor quality. An extremely thin face, especially one that is basically triangular, will have poor triangulation at its collapsed end. For example, here are two faces: one rectangular, one triangular When these two surfaces are meshed, the sharp triangular one will always have poor aspect ratio triangles at the sharp end.
Y ZX
V1
Y ZX Y ZX
8-2
Preparing Geometry for Meshing
As you will see in the example, in FEMAP the solution to this problem is to combine the adjacent surfaces and mesh them as one.
Suppressing Features A complex solid model may contain geometric features that are not significant enough to affect the analysis. In the example, you will suppress geometric features from the analysis without removing them from the geometric model. As a result, you can generate a much smoother mesh.
Preparing the Geometry To begin the example, you will import the geometry, then slice it in half since it is symmetrical.
Importing the Geometry What Start FEMAP and open a new model file. Import the Parasolid geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. BearingBlock.X_T Open OK
3.
View Style Menu (on View Toolbar) Choose Solid
4.
Rotate the model to an orientation similar to the following graphic.
Cutting the Geometry in Half
Step
UI
8-3
Command/Display
V1
ZY X
Cutting the Geometry in Half Since the part is symmetric, cut it in half to reduce meshing and analysis time. (Since this model is simple, you won’t save much time. However, this is an important technique for larger models.)
What Slice the symmetric part along the global ZX plane, at Y=1.
How Step
UI
Command/Display
1.
Geometry, Solid, Slice Menu
2.
Entity Selection dialog box: Double-click to select the solid.
Notice: Since there is only one solid, you can double-click to automatically select it and go to the next dialog box. 3.
Plane Locate dialog box: Methods
4.
Global Plane
5.
ZX Plane
8-4 Step
UI
Preparing Geometry for Meshing
Command/Display
6.
Y: 1 OK
V1
X 7.
ZY
Delete, Geometry, Solid Menu
8.
Entity Selection dialog box: Pick the +Y side of the solid. OK OK
V1
X
ZY
Creating New Boundary Surfaces To improve the quality of the mesh, combine some of the faces of the part to create larger boundary surfaces. The boundary surface defines an area to be meshed.
What Create boundary surfaces by combining each triangular face with the adjacent rectangular face.
Creating New Boundary Surfaces
How Step
UI
Command/Display
1.
View Style Menu (on View Toolbar) Choose Wireframe
2.
Geometry, Boundary Surface, From Surfaces on Solid Menu
3.
Entity Selection dialog box: Select one triangular face and the adjacent rectangular face. OK
4.
Select the two faces on the opposite side of the part. OK, then... Click Cancel Notice: You should now have two new boundary surfaces.
8-5
8-6
Preparing Geometry for Meshing
Suppressing Features Next, you will suppress the hole so that it will not be used in the meshing process.
What Suppress the hole.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Feature Suppression Menu
2.
Select Solid for Feature Suppression dialog box: OK Notice: Since there is only one solid, it is automatically selected.
3.
Feature Suppression dialog box: Manual
4.
Remove
5.
Loops
6.
Entity Selection dialog box: Pick a curve on the top or bottom of the hole.
Notice: When you pick loops, you pick a single curve at the top or bottom of a hole to suppress all faces underneath that loop in the topology of the solid.
Meshing the Model
Step
UI
8-7
Command/Display
7.
OK
V1
ZY X Notice: The surfaces are now gray, which means that they are suppressed. You may need to press Ctrl-G to see this change.
Meshing the Model Mesh the model using a large element size to keep the model under the 300-node demo license limit. If you have a full FEMAP installation, you might want to use a smaller element size to improve your results.
What Generate a solid mesh of the model. Set the element size to 0.5.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Define Material - ISOTROPIC dialog box: Load
3.
Select AISI 4340 Steel Click OK, then... OK again
4.
In Automesh Solids dialog box: Click Update Mesh Sizing...
8-8 Step 5.
UI
Preparing Geometry for Meshing
Command/Display In Automatic Mesh Sizing dialog box: Basic Curve Sizing: Element Size: 0.5 Click OK, then... In Automesh Solids dialog box: Click OK
V1
Z
6.
X
Y
Look in the Messages dockable pane to see information about the tet-meshing process.
Applying Loads and Constraints
Step
UI
8-9
Command/Display Notice: Your meshing diagnostic results may vary slightly from the values shown here. The key item in the diagnostics is the quality of surface triangles going into the tetrahedral mesher. Most of the triangles (98%) have aspect ratios between 1.0 and 2.0. The high quality surface mesh leads to high quality tetrahedral elements in the solid mesh.
Applying Loads and Constraints To prepare the model for analysis, apply a total vertical load to the top of the part. Fix the bottom of the part, and apply symmetric constraints.
What Apply a load of 10,000 pounds (5,000 pounds on the half symmetry model).
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set. OK 2.
Model, Load, On Surface Menu
3.
Entity Selection dialog box: Pick the top surface of the part. OK
4.
Create Loads on Surfaces dialog box: FX: 5000 OK
V1 L1
ZY X
8-10
Preparing Geometry for Meshing
What Apply a Y symmetry constraint along the symmetry cut that you made earlier. Fix the bottom of the part.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set. OK 2.
Model, Constraint, On Surface Menu
3.
Pick the surface that is the plane of symmetry. OK
4.
Create Constraints on Geometry dialog box Advanced Types: Surface
5.
Advanced Types: Sliding along Surface Click OK
6.
Pick the bottom two surfaces.
7.
Create Constraints on Geometry dialog box: Standard Types: Fixed OK
On Your Own
Step
UI
8-11
Command/Display
V1 L1 C1
ZY X
On Your Own Complete the analysis: solve the model with the NX Nastran static solver. Use the Model, Analysis command, create a new set, select “36..NX Nastran” as the Analysis Program and “1..Static” as the Analysis Type, click OK, then Analyze... button.
Once the analysis is complete, display a deformed and contour plot of T1 translation using one of the following methods: •
the View, Select command
•
the Post Data, Deformed, and Contour icons on the Post Toolbar. Also, look at the Post Options icon which contains many useful functions such as turning the “undeformed shape” on and off quickly.
•
the commands on the “context sensitive menu” of the Results branch of the Model Info tree (right click on the desired Results set to access the “context sensitive menu”).
This is the end of the example. You don’t need to save your model file.
8-12
Preparing Geometry for Meshing
9.
Repairing Sliver Geometry for Meshing In this example, you will learn to repair geometry for meshing. Slivers are small faces that are created because of numerical inaccuracies in Boolean or other solid modeling operations. Typically, these faces are much smaller than the other faces that define your solid. While they are small, they can cause great difficulties in meshing.
The example includes the following steps: •
importing the geometry with a missing sliver
•
stitching the surfaces
•
meshing the model
•
repairing problems with the geometry that caused the mesh to fail
•
meshing the new solid
Importing the Geometry What Start FEMAP and open a new model file. Import the Parasolid geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. Geometry_Repair.X_T Open OK
9-2 Step
UI
Repairing Sliver Geometry for Meshing
Command/Display
3.
View Style Menu (on View Toolbar) Choose Solid
4.
Rotate the model to an orientation similar to the following graphic.
V1
Y Z X Notice: The Parasolid file is imported as surfaces that need to be stitched together. The surfaces are assigned a random color. In this case, the sliver in the geometry is quite obvious, but often slivers are difficult to see.
Stitching the Surfaces Stitch the surfaces together to create a sheet solid, which is a type of Parasolid solid that has no volume. A sheet solid is basically a surface that you can use to perform solid surface operations, such as the Intersect, Stitch, Explode, and Slice commands.
What Stitch the surfaces back together.
How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
2.
Entity Selection dialog box: Select All OK (all dialog boxes)
Meshing the Model
Step
UI
9-3
Command/Display If FEMAP does not create a valid solid, it will temporarily turn all of the surfaces transparent, while highlighting and labeling the curves which were not stitched together.
The view will remain like this until a Window, Regenerate command has been performed using Ctrl+G or as part of another command, such as going from Solid to Wireframe using the View Style menu on the View Toolbar. Notice: The Messages dockable pane should also indicate that you’ve created a sheet solid. Tip: A sheet solid looks very similar to a regular solid. Follow the steps below to determine whether the model is a solid or a sheet solid. 3.
Tools, Mass Properties, Solid Properties Menu
4.
Select Solid for Mass Properties dialog box: Pick the solid from the list. OK No (don’t create a node and mass element), then OK for Density Notice: Examine the Messages dockable pane. If the volume has a value of 0, it is a sheet solid. If the volume has a value greater than 0, it is a regular solid. In this case, you have a sheet solid.
Meshing the Model Mesh the model containing the sliver.
What Mesh the solid model.
9-4
Repairing Sliver Geometry for Meshing
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Define Material - ISOTROPIC dialog box: Load
3.
Select From Library dialog box: Pick a material. OK (both Material dialog boxes)
4.
Automatic Mesh Sizing dialog box: OK Notice: FEMAP displays the message: “Mesher Aborted”. For more information about why the mesher failed, examine the messages in the Messages and Lists window. Tip: FEMAP first meshes the outside surface of the model. Then, based on the surface mesh, it meshes the inside volume with elements. The error message “Surface mesh has at least one hole” indicates that the tet mesher was not able to correctly mesh the surface. FEMAP aborted the meshing process and left the failed surface mesh on the model for diagnostic purposes.
5.
Tools, Undo Menu
Tip: Ctrl-Z is the shortcut for this command. Notice: Check the Messages dockable pane to make sure that you have undone the meshing command. If not, pick Undo until you have.
Repairing Problem Geometry Since meshing was aborted, you need to repair the geometry. First, try to use the geometry Cleanup command. If that doesn’t work, you’ll need to make manual repairs.
Running Cleanup
9-5
Running Cleanup The Geometry, Solid, Cleanup command checks the solid and removes any extraneous features that may have developed during export from a CAD package or from Boolean operations.
What Run the geometry Cleanup command to repair problems with the model.
How Step
UI
Command/Display
1.
Geometry, Solid, Cleanup Menu
2.
Entity Selection dialog box: Pick the solid. OK
3.
Solid Cleanup dialog box: Check the Remove Redundant Geometry, Remove Sliver Surfaces, and Check Geometry options (top three in dialog box). OK Notice: The Messages pane says that the solid has passed geometry checking. However, if you zoom and rotate the model, you will see that there is still a missing sliver.
Tip: Although the geometry passed the checker, you still may not be able to mesh it. Often, you will not be able to tell if a piece of geometry can be meshed without first trying to mesh it. With experience, you will learn what can be meshed and what needs to be modified. Before you mesh, try to visualize the size of the element and how the geometry could be constructed with it. If you can’t see how your geometry could be made from the elements, chances are the mesher won’t be able to, either.
Removing the Problem Geometry Since the geometry checker didn’t repair the geometry automatically, you will have to repair it manually. First, delete the problem surface, then create a new surface for the block.
What Explode the sheet solid into surfaces, then delete the surface that the sliver was removed from.
9-6
Repairing Sliver Geometry for Meshing
How Step
UI
Command/Display
1.
Geometry, Solid, Explode Menu
2.
Entity Selection dialog box: Pick the solid. OK
3.
Delete, Geometry, Surface Menu
4.
Entity Selection dialog box: Pick the surface that the sliver was removed from. OK, then... OK again to confirm the deletion
5.
Ctrl-G
Window, Regenerate
V1
Y Z X
Creating a New Surface Now that you have removed the problem geometry next to the sliver, you can create a new surface that can be meshed.
What When the curve was projected onto the face, the surface and the curve on one edge were split. Verify that there are two curves defining one edge.
Creating a New Surface
9-7
How Step
UI
Command/Display
1.
List, Geometry, Curve Menu
Move the cursor over the model to highlight the curves. Notice: One edge of the model will contain two curves (A and B, as shown in the figure).
A
B
What Run geometry Cleanup on the model to merge the curves. Use the new curve to create a new surface.
How Step
UI
Command/Display
1.
Geometry, Solid, Cleanup Menu
2.
Entity Selection dialog box: Select All OK
3.
Solid Cleanup dialog box: Check the Remove Redundant Geometry, Remove Sliver Surfaces, and Check Geometry options (top three in dialog box). OK
4.
Ctrl - G
5.
Window, Regenerate (the screen will verify that the curves were merged.) Geometry, Surface, Edge Curves
Menu
9-8 Step
Repairing Sliver Geometry for Meshing
UI
Command/Display
6.
Pick the four curves that made up the original surface. OK... then Cancel.
7.
Ctrl - G
Window, Regenerate
V1
Y Z X What Stitch the surfaces together.
How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
Stitch all surfaces together by clicking Select All, then... Clicking OK in all the dialog boxes Notice: Look at the Messages pane to verify that a solid was created. You can also doublecheck by using Tools, Mass Properties, Solid Properties.
Meshing the New Solid Now that you have repaired the problem geometry, you should be able to mesh it.
On Your Own
9-9
What Mesh the geometry.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
Use default values for meshing. Make sure that you load a material from the library.
On Your Own To complete the analysis: •
Apply a 100 psi pressure on the face that you corrected, and fix all of the corners.
•
Solve the model with the NX Nastran solver, using a “Linear Static” Analysis Type.
•
Display a contour of Solid von Mises Stress.
This is the end of the example. You don’t need to save your model file.
9-10
Repairing Sliver Geometry for Meshing
10.
Repairing a Mesh In this example, you will learn to repair a flawed mesh created from imported geometry.
V1
The FEMAP geometry import capability is very robust. From Parasolid systems, the capability is 100% reliable. From ACIS, IGES, STEP, Pro/ Engineer, and CATIA files, the reliability is very good. If the imported geometry contains problem surfaces, automatic meshing may not produce the best results. Sometimes it is easier to correct a bad mesh that results from bad geometry than it is to fix the bad geometry and then mesh it.
Z Y X The example includes the following steps: •
importing a flawed mesh
•
examining free edges to reveal the hole in the mesh
•
repairing the mesh problems
•
meshing the model again
Importing the Mesh What Start FEMAP and open a new model file. Import the neutral file containing the simple part with the flawed mesh.
How Step
UI
Command/Display
1.
File, Import, FEMAP Neutral Menu
2.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory. MeshFix.NEU Open OK
10-2 Step
UI
Repairing a Mesh
Command/Display
V1
Z Y X
Examining Free Edges Examine free edges to identify potential problems.
What Display free edges.
How Step
UI
Command/Display
1.
View Select (On View Toolbar)
2.
View Select dialog box: Model Style: Free Edge OK
3.
Zoom (on View Toolbar) Zoom in on the free edges.
V1
ZY X
Repairing Mesh Problems
10-3
Repairing Mesh Problems To repair the hole in the mesh, you’ll first create a group containing all the elements and free edge nodes. Next, you’ll manually create triangular mesh elements to fill the hole.
Creating a Group for Free Edge Nodes and Elements What Create a group containing the Free Edge nodes only.
How Step
UI
Command/Display
1.
Group, Set Menu
2.
Create or Activate Group dialog box: Title: Free Edge Nodes OK
3.
Group, Node, ID Menu
4.
Entity Selection dialog box: Method
5.
ID - Free Edge
6.
Entity Selection dialog box: Select the 5 nodes which are currently visible on the screen OK
What Add the elements using those “free edge” nodes to the group.
How Step 1.
UI
Command/Display View Select (On View Toolbar) or F5 key
10-4 Step
UI
Repairing a Mesh
Command/Display
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Group: Active OK (All dialog boxes) Tip: For a shortcut to the Model, Data command, right-click in the graphics region. From the menu, pick Model Data.
4.
Group, Element, using Node Menu
5.
Entity Selection dialog box: Choose 1..Free Edge Nodes from the Group drop-down list.
6.
Click OK
7.
Group, Operations, Automatic Add Menu
8.
Automatically Add to Group dialog box: Active OK Notice: You have now created a group containing the free edge nodes and the elements using the free edge nodes. We are concerned with the “hole” in the mesh.
Hole in Mesh
Creating New Plate Elements
10-5
Creating New Plate Elements What Create plot planar property, then new plate elements to fill the hole.
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Click Elem/Property Type button
3.
Element/Property Type dialog box: Choose Plot Only in the Plane Elements section
4.
OK, then... In Define Property dialog box: OK, then... Yes (to question), then... Cancel
5.
Model, Element Menu
6.
Define Plate Element dialog box: Triangle
7.
Nodes: Click in the first field, then pick three nodes to create a triangular element. OK Create 2 additional elements to close the hole, then click Cancel Note: As you create elements to fill the “hole”, the free edge gets smaller.
8.
View Select (On View Toolbar)
9.
View Select dialog box: Draw Model
10-6 Step
UI
Repairing a Mesh
Command/Display
10.
Model Data
11.
Select Model Data for View dialog box: Group: None OK (all dialog boxes)
Y Z X
Meshing the Model Now that you have closed the hole using plate elements, you can generate the tetrahedral mesh. The Solids from Elements command lets you create solids from elements without the underlying geometry.
What Mesh the model with tetrahedral elements.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids from Elements Menu
2.
Entity Selection dialog box: Select All OK In Define Material - ISOTROPIC dialog box: Load
Meshing the Model
Step
UI
3.
Command/Display Select from Library dialog box: Select any material from the library
4.
OK, then... In Define Material - ISOTROPIC dialog box: OK, then... In Automesh Solids dialog box: OK
5.
Ctrl-A
Autoscale the model.
This is the end of the example. You don’t need to save your model file.
10-7
10-8
Repairing a Mesh
11.
Analyzing a Beam Model
In this example, you’ll use rod and L beam elements to represent a truss structure.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the truss
•
defining the material and property
•
meshing the model using beams and rods
•
applying constraints and loads
•
analyzing the model using NX Nastran
•
post-processing the results
Importing the Geometry What Open a new model file and import the geometry of the truss. These curves will be meshed with rod and beam elements.
How Step
UI
Command/Display
1.
File, Import, FEMAP Neutral Menu
2.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory. Truss.NEU Open OK
11-2 Step
UI
Analyzing a Beam Model
Command/Display
Y
X Z
Defining the Material and Property The first step for the meshing process will be to define the material and property for the beam and rod elements.
Defining the Material What Define the material by selecting a standard material from the FEMAP material library.
How Step
UI
Command/Display
1.
Model, Material Menu
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). 2.
Define Material - ISOTROPIC dialog box: Load
3.
Select from Library dialog box: AISI 4340 Steel OK OK, then... Cancel
Defining the Beam Property FEMAP has a library of general cross sections for you to choose from, but you may not always want to use them. You can define an arbitrary cross section by creating a surface in FEMAP, or by importing external geometry. FEMAP will then calculate the section properties from that surface.
Defining the Beam Property
11-3
The neutral file that you imported has a boundary surface on a different layer that is not currently shown. You will now display it.
What First, hide the default layer. Next, display the boundary surface on a hidden layer.
How Step
UI
Command/Display
1.
View, Layers Menu
Tip: You can also pick the Layers icon
on the View Toolbar to open this dialog box.
You can also use the Manage command from the “context sensitive menu” located on the Layers branch in the Model Info tree (simply click to highlight any Layer, then right mouse click to see the context sensitive menu). 2.
Layer Management dialog box: Visible Layers: Default Layer
3.
Click Hide
4.
Hidden Layers: Beam Section
5.
Click Show OK
6.
Ctrl - A
Autoscale Notice: The boundary section and curves are displayed.
Y
X Z
11-4
Analyzing a Beam Model
What Define a property for the beam elements. You’ll first create a general beam cross section, then define a vector to define the section’s Y axis. Next, you’ll define the beam property with the cross section and the AISI 4340 material that you’ve created.
How Step
UI
Command/Display
1.
Model, Property Menu
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). 2.
Define Property dialog box: Elem/Prop Type
3.
Element Property Type dialog box: Line Elements: Beam OK
4.
Define Property dialog box: Shape
5.
Cross Section Definition dialog box: Shape: General Section
6.
Surface
7.
Select Surface to Check dialog box: Click on the surface. OK
8.
Vector Locate - Define Section Y Axis dialog box: Base: 0, 0, 0 (make sure these are the X,Y,Z values for the base) Tip: 0, 1, 0 (enter these X,Y,Z values for the tip) OK Notice: This vector defines the Y axis for the section.
9.
Cross Section Definition dialog box: OK
Meshing the Model
Step
UI
10.
11-5
Command/Display Define Property dialog box: Title: General Beam Section Notice: The calculated section properties are now displayed in this dialog box.
11.
Material: AISI 4340 Steel OK, then... Cancel
Meshing the Model This model will be meshed with two types of elements: beam elements on the longitudinal curves, and rod elements on the curves that connect the beams. Once you’ve created the elements, you’ll merge the coincident nodes.
Creating the Beam Mesh First, mesh the longitudinal curves with beams whose properties were defined in the previous section.
What Hide the beam section and show the default layer.
How Step
UI
1.
Command/Display Layers (on View Toolbar)
Tip: You can also “Hide and Show” layers directly from the Layers branch in the Model Info tree. Simply pick on any number of layers (hold down the Ctrl or Shift key to select Multiple layers), then choose the Hide or Show command from the “context sensitive menu”. 2.
Layer Management dialog box: Hide the Beam Section, and show the Default Layer. OK
3.
Ctrl - A
Autoscale
11-6 Step
UI
Analyzing a Beam Model
Command/Display V1
Y
X Z
What Rotate the model to get a trimetric view for meshing.
How Step
UI
Command/Display
1.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 2.
View Rotate dialog box: Trimetric OK
What Mesh the longitudinal curves with beams. You’ll use the general beam cross section to define the beam. After you select the cross section, you’ll enter a vector to define the beam element orientation. It’s important that this vector be identical to the one used to define the cross section properties; otherwise, your analysis results may be incorrect.
How Step
UI
Command/Display
1.
Mesh, Geometry, Curve Menu
2.
Entity Selection dialog box: Pick the curves highlighted in the following figure. OK
Creating the Beam Mesh
Step
UI
3.
Command/Display
Geometry Mesh Options dialog box: Property: General Beam Section OK
4.
Vector Locate dialog box: Base: 0, 0, 0 (make sure these are the X, Y, Z values for the base) Tip: 0, 1, 0 (enter these X, Y, Z values for the tip) OK V1
Y X Z
What Display the beam elements with their cross sections visible.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Element Orientation/Shape (select) Element Shape: Show Cross Section (select) OK
11-7
11-8 Step
UI
Analyzing a Beam Model
Command/Display
Tip: You can also “toggle” the cross-sections of line elements on/off using the “Thickness/ Cross Section” command from the View Style menu located on the View Toolbar.
What Rotate and zoom the model to get a better look at the cross section. Your cross section may have an incorrect orientation that you need to modify.
How Step
UI
Command/Display
1.
Rotate the model slightly to the see the cross sections better.
2.
Zoom (on View Toolbar)
Notice: Compare your beams with the following diagram. Note that the “notch” on each cross section faces the inside of the part. If some of your beams are oriented differently, you will need to modify them. The following steps show you how to reverse the normals when they are facing in the wrong direction. It is normal for you to need to modify the normal direction of some of your beams to make it look like the figure below.
Creating the Rod Mesh
Step
UI
11-9
Command/Display
3.
Modify, Update Elements, Line Element Reverse Direction Menu
4.
Entity Selection dialog box: Pick the elements to modify. (Pick only the elements with cross sections facing in the wrong direction.) OK
5.
Ctrl - A
Autoscale
Creating the Rod Mesh You will now mesh the remaining curves with rod elements to connect the beams.
What Mesh the curves. You’ll also need to create a new property to define the rods.
11-10
Analyzing a Beam Model
How Step
UI
Command/Display
1.
Mesh, Geometry, Curve Menu
2.
Entity Selection dialog box: Pick all of the unmeshed curves: the cross braces and the connection between the two rows of beams. OK
3.
Geometry Mesh Options dialog box: New Prop Notice: You only have the General Beam Section property in your model. You’ll need to create a rod property.
4.
Define Property dialog box: Elem/Property Type
5.
Line Elements: Rod OK
6.
Define Property dialog box: Title: 2 in Diam Rod
7.
Area: 3.14
8.
Material: AISI 4340 Steel OK
9.
Geometry Mesh Options dialog box: OK Notice: The property you created is selected for the element’s property. Notice: The curves are meshed with rod elements.
Merging Coincident Nodes
Step
UI
11-11
Command/Display
What Reduce the amount of information displayed by turning off the display of geometry and labels.
How Step
UI
Command/Display
1.
Ctrl - Q
View Quick Options dialog box:
Notice: You can also turn on this dialog box with the Quick Options toolbar icon 2.
Geometry Off Labels Off Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry and Labels on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. The third icon allows you to toggle Labels on and off.
Merging Coincident Nodes Because the curves were meshed with two meshing operations, there will be nodes at the ends of both the beam and rod elements. You will merge these coincident nodes to effectively “sew” the model together.
What Merge the coincident nodes.
11-12
Analyzing a Beam Model
How Step
UI
Command/Display
1.
Tools, Check, Coincident Nodes Menu
2.
Entity Selection dialog box: Select All OK
3.
Check/Merge Coincident dialog box: Options: Merge Coincident Entities (check) OK Notice: Look in the Messages dockable pane to see how many coincident nodes have been merged. All rod and beam elements are now connected together.
Applying Constraints and Loads You will create a constraint set to model symmetry and fix the end. The symmetry of the truss will be used to reduce the model to half the size. You will also apply a load to this model to simulate something hanging from the truss.
Modeling Symmetry and a Fixed End To simulate the symmetry of this part, you will constrain the four nodes that are at the halfway point of the structure. You are defining symmetry across the X-plane through these four points. By imposing this type of constraint condition, you are actually introducing a stiffness exactly equal to the structure modeled, just mirrored above the X-plane.
What Create the constraints to model symmetry and fix the end. You’ll also constrain the rest of the model in all DOF except the X and Y translations.
How Step
UI
Command/Display
1.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 2.
View Rotate dialog box: Isometric OK
Modeling Symmetry and a Fixed End
Step
UI
11-13
Command/Display
3.
Model, Constraint, Nodal Menu
Notice: First, you’ll apply constraints at these nodes to model symmetry. 4.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
5.
Entity Selection dialog box: Pick nodes A, B, C, and D (see the following figure). OK
A D B C 6.
Create Nodal Constraints/DOF dialog box: X Symmetry OK Notice: The TX, RY, and RZ DOF are selected. Because you are applying nodal constraints, you could control the constraint of each degree of freedom individually in the dialog box, or you can use the quick keys to apply common constraint conditions.
7.
Entity Selection dialog box: Pick nodes E and F (see the following figure). OK Notice: You are now fixing the nodes on the opposite end.
11-14 Step
UI
Analyzing a Beam Model
Command/Display F E
8.
Create Nodal Constraints/DOF dialog box: Fixed OK Notice: All DOF are selected.
9.
Entity Selection dialog box: Select All OK Notice: Finally, you’ll restrain the DOF for all nodes in the Z translation and all rotations.
10.
Create Nodal Constraints dialog box: DOF: TZ, RX, RY, RZ (check) OK
11.
No (to combine the constraints)
What Turn off element cross sections to better see the constraints.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Element Orientation/Shape (select) Element Shape: Line/Plane Only (select) OK
Applying a Load to the Model
Step
UI
11-15
Command/Display
Tip: If you turn the constraint labels back on, you’ll see the degree of freedom numbers displayed for each constraint. (To do this, pick F6. Pick Options, Constraint. Under Label Mode, pick Degree of Freedom.)
Applying a Load to the Model You will now apply a load in the negative Y direction to simulate something hanging from this truss. Like constraints, loads are grouped in sets. Before creating any loads, you must create a set to hold them.
What Create the load in the negative Y direction.
How Step
UI
Command/Display
1.
Model, Load, Nodal Menu
2.
Create or Activate Load Set dialog box: Title: (enter a title) OK
3.
Entity Selection dialog box: Pick nodes A and B. OK
11-16 Step
UI
Analyzing a Beam Model
Command/Display
B A
4.
Create Loads on Nodes dialog box: FY: Value: -200 OK Notice: The default load type is force.
Analyzing the Model Analyze the model using the NX Nastran solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: New
Post-Processing the Results
Step
UI
11-17
Command/Display
3.
Analysis Set dialog box: Title: (enter a title for the solve)
4.
Analysis Program: 36..NX Nastran Analysis Type: 1..Static OK
5.
Analyze
Post-Processing the Results For this example, you will display two types of results: criteria plots and beam diagrams.
Displaying Criteria Diagrams As an alternative to contours, you can use a basic criteria display that shows the output value of each element. The primary purpose of a criteria display, however, is to limit the display based on a selected criteria.
What Display a basic criteria view of the results.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform
3.
Contour Style: Criteria
4.
Deformed and Contour Data
5.
Select PostProcessing Data dialog box: Output Vectors: Deformation: Total Translation Contour: 3022..Beam EndA Axial Force OK (all dialog boxes)
6.
View, Rotate, Model Menu
11-18 Step
UI
Analyzing a Beam Model
Command/Display Tip: You can press the F8 key instead of using the command above.
7.
View Rotate dialog box: Trimetric OK
What To reduce clutter, turn off display of undeformed elements.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Category: PostProcessing
3.
Options: Undeformed Model
4.
UNCHECK Draw Entity OK
Displaying Criteria Diagrams
Step
UI
11-19
Command/Display
What Modify the criteria for the elements to be displayed. Display the elements above the maximum limit of 350.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Notice: The PostProcessing category is already selected.
3.
Options: Criteria Limits
4.
Minimum: 0 Maximum: 350
5.
Limits Mode: Above Maximum OK
Notice: Only the elements with axial force values above 350 are displayed as shaded beams; the other elements don’t have color.
11-20 Step
UI
Analyzing a Beam Model
Command/Display
Displaying Beam Diagrams To conclude the example, you’ll generate beam diagrams of the axial stress. Beam diagrams display results along the length of line elements. You can set options to control the direction of beam diagrams.
What Generate a beam diagram of beam end axial stress.
How Step
UI
Command/Display
1.
View Select (On View Toolbar)
2.
View Select dialog box: Deformed Style: None - Model Only Contour Style: Beam Diagram
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Contour: 3139..Beam EndA Pt1 Comb Stress OK (all dialog boxes)
Displaying Beam Diagrams
Step
UI
11-21
Command/Display
What You can change the plane where the beam diagram will be drawn. FEMAP always draws the diagram in the plane that you choose, even if the output is actually based on forces/stresses in a different plane.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Options: Beam Diagram Default Direction: Element Z OK Notice: The beam diagrams are now drawn on the element Z plane.
11-22 Step
UI
Analyzing a Beam Model
Command/Display
This is the end of this example. You don’t need to save the model file.
12.
Analyzing an Axisymmetric Model In this example, you will take advantage of the axisymmetric nature of a pressure vessel and analyze the part using axisymmetric elements. The example includes the following steps: • importing the geometry • meshing the model • applying constraints and loads • analyzing the model using NX Nastran • post-processing the results
Importing the Geometry To begin the example, you will import the geometry of a pressure vessel that was created in AutoCAD. The geometry was exported from AutoCAD as an AutoCAD DXF file. DXF files are popular for transferring geometry between CAD programs and desktop publishing software.
What Start FEMAP and open a new model file. Import the geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. Vessel.DXF Open OK
12-2 Step
Analyzing an Axisymmetric Model
UI
Command/Display
V1
Y ZX
Meshing the Model You will first set the global mesh size, then define the materials and properties for the mesh. Next, you will create a boundary surface and mesh the part.
Setting the Global Mesh Size As the first step in the meshing process, you will set the global mesh size then view it to verify that mesh spacing is appropriate.
What Set the global mesh size.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Default Size Menu
2.
Default Mesh Size dialog box: Size: 0.25 OK
3. 4.
F6 key
View Options View Options dialog box: Curve - Mesh Size Show As: 2..Symbols (all curves) OK
Creating the Material and Property
Step
UI
12-3
Command/Display Notice: You should see small dots/diamonds along each of the geometric entities in FEMAP. These dots/diamonds indicate where nodes will be created during any automatic meshing commands that use this geometry.
V1
Y Z X
Creating the Material and Property Create the material and property for the elements.
What Create the material by selecting a standard material from the FEMAP material library.
How Step
UI
Command/Display
1.
Model, Material Menu
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). 2.
Define Material - ISOTROPIC dialog box: Load
3.
Select from Library dialog box: 15-5PH Stainless H1025 (select) OK OK, then... Cancel
12-4
Analyzing an Axisymmetric Model
What Create the property for the axisymmetric mesh elements.
How Step
UI
Command/Display
1.
Model, Property Menu
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). 2.
Elem/Property Type
3.
Element Property Type dialog box: Volume Elements: Axisymmetric OK
4.
OK to show Axisymmetric Axis in all Views: Yes
5.
Define Property dialog box: Title: Axisymm 15-5PH
6.
Material: 15-5PH Stainless H1025 OK, then... Cancel
What Correct the axisymmetric axis orientation. This axis gives a visual cue to the orientation of the model and for axisymmetric shell elements, provides the axis used to define load direction.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Category: Tools and View Style
Meshing the Model
Step
UI
12-5
Command/Display
3.
Options: Axisymmetric Axes
4.
Direction: Global Y, X Radial OK
Meshing the Model This shape could be broken down into simple geometric regions for mapped meshing, but it is much easier to create a FEMAP boundary surface and automatically mesh the whole part.
What Create a boundary surface.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select All OK, then... Cancel
V1
Y ZX What Generate a mesh of the model.
12-6
Analyzing an Axisymmetric Model
How Step
UI
Command/Display
1.
Mesh, Geometry, Surface Menu
2.
Entity Selection dialog box: Pick the boundary. OK
3.
Automesh Surfaces dialog box: Property: Axisymm 15-5PH Stainless H1025
4.
Element Shape: All Triangles
5.
Fast Tri-Mesh (turn on - if not on by default) OK
6. 7.
Ctrl-Q
View Quick Options View Quick Options dialog box: Geometry Off Labels Off Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry and Labels on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. The third icon allows you to toggle Labels on and off.
Applying Constraints and Loads
Step
UI
12-7
Command/Display
V1
Y ZX
Applying Constraints and Loads To prepare the model for analysis, constrain the base of the model, and apply a pressure load. Since this model is axisymmetric, there is no need to apply any constraints on loads out of plane.
Defining Constraints What Constrain the bottom nodes along the flat edge against vertical movement.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set. OK 2.
Model, Constraint, Nodal Menu
3.
Entity Selection dialog box: Pick the four nodes along the bottom of the part (see following figure). OK
12-8 Step
Analyzing an Axisymmetric Model
UI
Command/Display
V1 L1 C1
Y Z X 4.
Create Nodal Constraints/DOF dialog box: TY OK
V1 L1 C1
Y ZX
Defining Loads In an axisymmetric model, a pressure load is applied to the edges of the axisymmetric elements. Since the load is applied to the edges of the elements, FEMAP requires you to specify the element and which face of the element gets the load. Here you will use the Adjacent Faces method to apply loads to the model.
What Apply a pressure load to the interior faces of the elements.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set. OK 2.
Model, Load, Elemental Menu
Defining Loads
Step 3.
UI
12-9
Command/Display Entity Selection dialog box: Select All OK
4.
Create Loads on Elements dialog box: Pressure: Value: 100 OK Tip: In this example, you are applying a pressure load to edges. However, if you wanted instead to apply a nodal force load to an axisymmetric model, some solvers require that you define the load data as force/length/radian, while others use force/length/degree. Be sure to check your analysis software’s documentation to verify which convention is appropriate.
5.
Face Selection for Elemental Loads dialog box: Method: Adjacent Faces
6.
Face (click in field) Notice: Clicking in this field moves the focus (the flashing cursor) there. When you select from the Graphics window, FEMAP will know that you are trying to pick a face.
7.
Pick an element face on the inside of the part.
V1 L1 C1
Y ZX 8.
Tolerance: 85 OK Notice: The Adjacent Faces method selects connected free faces (edges, in this case) until it finds a connected free face that exceeds the angle tolerance. In this example, by entering a very large angle tolerance of 85 degrees, the software selects all the internal faces up to the corners along the Y axis. To go around this corner, you would need to enter an angle of 90 degrees or greater.
12-10 Step
UI
Analyzing an Axisymmetric Model
Command/Display
Analyzing the Model Solve the model using the NX NASTRAN solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Create an analysis set.
2
Select the “36..NX Nastran” from the Analysis Program drop down menu Select “1..Static” from the Analysis Type drop down menu. Use all default values.
3.
Analyze
4.
Yes (verify that it’s OK to flip the model) Yes again (force all element normals to lie along the correct global axis)
Post-processing the Results
Step
UI
12-11
Command/Display Tip: NX Nastran also makes the following assumptions for an axisymmetric model:
5.
•
The Z axis is the axis of symmetry.
•
The X axis is in the radial direction.
•
All nodes must lie in the X-Z plane of the global coordinate system, and must have a nonnegative X (radial) coordinate.
•
All loads must be in the X-Z plane.
•
The Y axis of all nodal displacement coordinate systems must be parallel to the global Y axis.
•
XY and YZ shear stresses and strains are zero.
•
All gravity vectors must be parallel to the axis of symmetry.
•
All angular velocity vectors must lie on the axis of symmetry.
Scale Factor for Axisym Forces dialog box: OK Tip: The scale factor does not affect the pressures that you defined for this example. However, if you define nodal forces for an axisymmetric model, the scale factor lets you convert nodal load values for use with a different solver. For instance, suppose that you have defined a nodal force value for a solver that uses units of force/length/degree. To analyze the model with a different solver, you can use the scale factor to convert the nodal load value to units of force/length/radian.
6.
Yes (To permanently convert the elements to triangular elements with midside nodes) Yes again (to save the model so you can view the results in the correct model)
Post-processing the Results For this analysis, you will display deformation and stress contours.
What Display and deformed/contour plot of translation and Azimuth (hoop) stress for the pressure vessel part.
How Step
UI
Command/Display
1.
F8 key
View Rotate Model
2.
View Rotate dialog box: ZX Front OK
12-12 Step
UI
Analyzing an Axisymmetric Model
Command/Display
V1 L1 C1
Z Y X 3.
F5 key
4.
View Select View Select dialog box: Deformed Style: Deform Contour Style: Contour
5.
Deformed and Contour Data
6.
Select PostProcessing Data dialog box: Output Vectors: Deformation: 1. Total Translation Output Vectors: Contour: 6029: Axisym Azimuth Stress OK (all dialog boxes)
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
8.
In View Quick Options dialog box:
UNCHECK Node box located in the Geometry section, then
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Nodes on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
Post-processing the Results
Step
UI
Command/Display
9.
F6 key
View Options
10.
View Options dialog box: Category: PostPorcessing
11.
Options: Undeformed Model
12.
Draw Entity: OK
This is the end of the example. You don’t need to save your model file.
12-13
12-14
Analyzing an Axisymmetric Model
13.
Analyzing a Midsurface Model of a Welded Pipe
In this example, you will model a welded pipe to determine the force distribution along the weld line between the two tubes. L O A D
Fixed
Fixed
To use this model with the 300-node demonstration version, you will model a midsurface shell mesh on a quarter of this part, then use symmetrical boundary conditions to represent the remaining three-quarters of this model. The example includes the following steps: •
importing the geometry using the Parasolid interface
•
slicing the model
•
creating the midsurface model
•
meshing the model
•
applying loads and constraints
•
analyzing the model using NX Nastran
•
post-processing the grid-point force balance results using Freebody Display
Importing the Geometry To begin the example, you will import the geometry.
What Start FEMAP and open a new model file. Import the Parasolid geometry file.
13-2
Analyzing a Midsurface Model of a Welded Pipe
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the Examples directory. Import the Pipe.X_T file. 2.
Solid Model Read Options dialog box: OK
3.
Rotate the model to the orientation shown.
V1
Y X Z
Slicing the Model Slice the model so that the -X quarter remains.
What Slice through the XY global axis at Z=5.0. Next, slice the model through the global YZ axis at X=0.0.
How Step
UI
Command/Display
1.
Geometry, Solid, Slice Menu
2.
Entity Selection dialog box: Pick the solid. OK
Slicing the Model
Step
UI
Command/Display
3.
Plane Locate dialog box: Methods
4.
Global Plane
5.
XY Plane
6.
Z: 5.0 OK
7.
Geometry, Solid, Slice Menu
Select the +Z solid (Solid on right in view below). Slice the solid along the YZ global plane at X = 0.0.
V1
Y X Z What Delete the -Z half and +X quarter of the model.
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
13-3
13-4 Step
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
2.
Entity Selection dialog box: Pick the -Z half of the model. (Solid on left in above figure) OK OK
3.
Delete, Geometry, Solid Menu
Delete the +X half of the model.
V1
Y X Z
Creating the Midsurface Model Create the midsurface model, then delete the original solid. Stitch the unconnected surfaces together to form one piece of geometry.
Creating the Midsurface What Use the automatic midsurfacing capability to create a midsurface model.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Automatic Menu
2.
Entity Selection dialog box: Select All OK
Creating the Midsurface
Step
UI
3.
13-5
Command/Display Midsurface Tolerance dialog box: Move the cursor to the Graphics window.
4.
Ctrl-D Notice: The Ctrl-D command lets you determine distance for the target thickness. The software uses this value to determine which surfaces to place a midsurface between. The target thickness should be slightly larger than the largest distance between the planes on the solids that you want midsurfaced. If the target thickness is too low, the midsurfaces will not be created. If the target thickness is too high, some midsurfaces will be created between the wrong surfaces.
5.
Locate dialog box: Methods
6.
On Point
7.
Move the cursor to the Graphics window. Snap to Point
8.
On Point dialog box: Pick point A (see following figure). OK Note: If you have trouble picking, click in the Point ID field to reset the picking focus.
V1
A B
X YZ 9.
Pick point B. OK
13-6 Step
Analyzing a Midsurface Model of a Welded Pipe
UI
Command/Display
10.
Midsurface Tolerance dialog box: OK (accept the value calculated by the Ctrl-D command) Notice: The target thickness value should be approximately 0.1.
Tip: The Geometry, Midsurface, Automatic command is actually a combination of three commands: (1) Geometry, Midsurface, Generate; (2) Geometry, Midsurface, Intersect; and (3) Geometry, Midsurface, Cleanup. If the Automatic command has removed necessary midsurfaces, you can work through the midsurfacing commands one at a time, so that you can more easily pick which surfaces should be kept.
Deleting the Solid What Delete the original solid.
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
2.
Entity Selection dialog box: Pick the solid. OK OK
Stitching the Geometry
Step
UI
13-7
Command/Display
V1
Y XZ
Stitching the Geometry Connect the three surfaces together into one piece of geometry.
What Stitch the three surfaces together. How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
2.
Entity Selection dialog box: Select All OK
3.
Surface/Solid Stitching dialog box: OK You will notice that the model will become transparent and the curves which were not stitched together will be highlighted and labeled. This lets you know all of the internal surfaces are now part of the same sheet solid.
13-8
Analyzing a Midsurface Model of a Welded Pipe
Meshing the Model The first step in meshing the model is to assign mesh attributes for the different surfaces. If the correct attributes are not assigned, the results won’t be accurate. Next, set the size for the mesh. Finally, mesh the midsurface.
Assigning Mesh Attributes What Assign the mesh attributes to the surfaces.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Assign Mesh Attributes Menu
2.
Entity Selection dialog box: Select All OK
3.
Define Material - ISOTROPIC dialog box: Load
4.
AISI 4340 Steel OK (all dialog boxes)
Notice: Each surface now has a material property assigned to it.
Meshing the Model What Set the mesh size to the default value, and mesh the model.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
Meshing the Model
Step
UI
13-9
Command/Display
2.
Entity Selection dialog box: Select All OK
3.
Automatic Mesh Sizing dialog box: Element Size: 0.3 OK Note: FEMAP will display small diamonds that indicate the mesh seed locations along the edges of the surfaces being meshed.
4.
Mesh, Geometry, Surface Menu
5.
Entity Selection dialog box: Select All OK
6.
Automesh Surfaces dialog box: OK Note: The Property field is filled in with “Use Meshing Attributes”.
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
13-10 Step
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
8.
In View Quick Options dialog box:
UNCHECK Surface box located in the Geometry section, then
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Surfaces on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
Applying Loads and Constraints You will apply a load that represents 1000 pounds vertical. Since the model is symmetric, you’ll also need to apply constraints to define this symmetry. What Apply a load that represents 1000 pounds vertical (+Y). Since you have modeled only one-quarter of the part, you need to apply a load of 250 to the top curve.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Applying Loads and Constraints
Step
UI
Command/Display
2.
Create or Activate Load Set dialog box: Title: (enter a title) OK
3.
Model, Load, On Curve Menu
4.
Entity Selection dialog box: Pick the top curve as shown in the following figure. OK
5.
Create Loads on Curves dialog box: FY: 250 OK
13-11
13-12
Analyzing a Midsurface Model of a Welded Pipe
What Apply nodal constraints to the symmetric edges, and fix one edge of the part.
X Symmetry
Z Symmetry
Z Symmetry Fixed
X Symmetry
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Model, Constraint, Nodal Menu
3.
Entity Selection dialog box: Method
4.
On Curve
5.
Pick the two curves shown below. OK
Applying Loads and Constraints
Step
6.
UI
Command/Display
Create Nodal Constraints/DOF dialog box: Z Symmetry OK
7.
Entity Selection dialog box: Pick the three curves shown in the following figure. OK
8.
Create Nodal Constraints/DOF dialog box: X Symmetry OK No (to combine, not overwrite)
9.
Entity Selection dialog box: Pick the curve shown in the following figure. OK
13-13
13-14 Step
UI
10.
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
Create Nodal Constraints/DOF dialog box: Fixed OK No (to combine, not overwrite)
11. 12.
Crtl-Q
This will bring up View Quick Options dialog box: In View Quick Options dialog box: Labels Off Click Done
Analyzing the Model Solve the model using the NX Nastran solver.
What Create the analysis set and solve the model.
Post-processing the Results
13-15
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: Create a new analysis set. Select the “36..NX Nastran” from the Analysis Program drop down menu Select “1..Static” from the Analysis Type drop down menu. OK
3.
Master Requests and Conditions (double-click to expand) Output Requests (select)
4.
Edit
5.
Output Requests dialog box: Nodal: Force Balance (check)
6.
In the Customization portion of the dialog box select: Results Destination: 2..PostProcess Only Notice: Using “2..PostProcess Only” will force NX Nastran to create output in a binary file (.op2 file) instead of in the print file (.f06 file). The .f06 file does not contain the Grid Point Force data required for FEMAP to create a Freebody Diagram. Also, “3..Print and Post” can not be used to retrieve Grid Point Force data. This is because FEMAP always reads in the .f06 file first to attain any error, warning, and information messages. If the .f06 contains output, FEMAP will read that output in and skip the read of the .op2 file. Tip: When you pick the force balance option, NX Nastran will output all the forces that act on each node of the model from all elements connected to that node. With this information, you can create a freebody diagram of the model or any portion of the model.
7.
Click OK, then... Click Analyze
Post-processing the Results For this analysis, you will generate a freebody display. You will first group the elements in the model to split it along the weld line. You can then view a freebody diagram of part of the model, thus displaying forces along the weld.
What Create a group of the nodes and elements of the lower surface.
13-16
Analyzing a Midsurface Model of a Welded Pipe
How Step
UI
Command/Display
1.
Group, Set Menu
2.
Create or Activate Group dialog box: ID: 2 Title: Lower Surface OK Notice: Group 1 was automatically created when you generated midsurfaces.
3.
Group, Element, On Surface Menu
4.
Entity Selection dialog box: Pick the lower surface. OK
5.
Group, Node, On Surface Menu
6.
Entity Selection dialog box: Pick the lower surface. OK
7.
Grp (click on the Status bar at the bottom of the FEMAP window)
Post-processing the Results
Step
UI
8.
13-17
Command/Display Pick Group 2 to make it active.
Notice: The Status bar lists the active group (for example, Grp:2). 9.
Grp (Status bar)
10.
View Active
Tip: You can also manage groups using the Model Info tree. Double click on any group to make it the “Active” group and you can toggle on and off the View Active command using the “context-sensitive menu” available by right-clicking on any Group. There many other functions which can be performed with the “context-sensitve menu” for Groups.
What Generate a freebody display.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Select PostProcessing Data dialog box: Freebody Display
4.
View Freebody Options dialog box: Freebody Style: Show Freebody Display (check)
5.
Freebody Group: Active (turn on)
13-18 Step 6.
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display Freebody Options: Show Forces (check) Show Moments (turn off) Entity Colors (check) Show Load Summation (check) Show Freebody on All Internal Nodes (turn off) Scale Vectors by Magnitude (turn off) Minimum Vector Magnitude (check) Display Vector Components (check) Y (check) X and Z (turn off) OK (all dialog boxes)
Notice: Since you are only viewing Y components of force, you see the vertical reaction forces at the fixed end of the part as well as the vertical load transfer through the nodes at the welded interface. Note the variation in vertical load transfer through the welded connection. Calculating an effective length for a node with the highest force (99.852 pounds) indicates a running load of approximately 359.5 pounds/inch. If you were to assume an equal distribution of load along the joint, the running load would have been 17.7 pounds per inch. This is the end of the example. You don’t need to save your model file.
14.
Analyzing a Midsurface Model of an Electrical Box In this example, you will learn to work with FEMAP’s semi-automatic midsurface extraction capabilities to build an idealized model of an electrical box. To work through this example, you must have a licensed copy of NX Nastran for FEMAP. You will not be able to complete this example with the 300-node demo version.
The example includes the following steps: •
importing the geometry using the STEP interface
•
creating the midsurface model
•
meshing the model
•
applying loads and constraints
•
analyzing the model using NX Nastran
•
post-processing the results
Importing the Geometry To begin the example, you will import the geometry.
What Start FEMAP and open a new model file. Import the STEP file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the Examples directory. Import the mp.STP file. 2.
STEP Read Options dialog box: OK
14-2 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
3.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 4.
View Rotate dialog box: Dimetric OK
5.
View Style Menu (on View Toolbar) Choose Wireframe
Creating the Midsurface Model Create the midsurface model, then delete the original solid. Once the midsurface has been generated, you will need to so some additional cleanup work on the geometry before you can mesh it.
Creating the Midsurface What Use the automatic midsurfacing capability to create a midsurface model.
How Step 1.
UI
Command/Display Zoom and rotate the part to get a better view of the points we will be picking to designate the “Target Distance” for midsurfacing.
Creating the Midsurface
Step
UI
14-3
Command/Display
2.
Geometry, Midsurface, Automatic Menu
3.
Entity Selection dialog box: Select All OK
4.
Midsurface Tolerance dialog box: Move the cursor to the Graphics window.
5.
Ctrl-D Notice: The Ctrl-D command lets you determine distance for the target thickness. The software uses this value to determine which surfaces to place a midsurface between. The target thickness should be slightly larger than the largest distance between the planes on the solids that you want midsurfaced. If the target thickness is too low, the midsurfaces will not be created. If the target thickness is too high, some midsurfaces will be created between the wrong surfaces.
6.
Locate dialog box: Methods
7.
On Point
8.
On Point dialog box: Pick point A (see following figure). OK
14-4 Step
Analyzing a Midsurface Model of an Electrical Box
UI
Command/Display
V1
A B
ZY X 9.
Pick point B. OK
10.
Midsurface Tolerance dialog box: OK (accept the value calculated by the Ctrl-D command) Notice: The target thickness value should be approximately 4.9.
V1
Z Y X
Deleting the Solid What Delete the original solid.
Cleaning Up the Geometry
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
2.
Entity Selection dialog box: ID: 1 OK OK
3.
View Style Menu (on View Toolbar) Choose Solid
Cleaning Up the Geometry To create a more accurate midsurface model, you must trim each rib, then delete the top portion.
What Trim the surface of each rib.
14-5
14-6
Analyzing a Midsurface Model of an Electrical Box
How Step
UI
Command/Display
1.
Geometry, Midsurface, Trim with Curve Menu
2.
Select Surface/Solid to Trim dialog box: Pick one of the eight ribs. OK
C
3.
Entity Selection dialog box: Pick the curve on the lower portion (see C above). OK Notice: The curve now cuts through the surface.
V1
Z Y X 4.
Repeat the process to trim the other seven ribs.
Cleaning Up the Geometry
Step
UI
14-7
Command/Display Tip: When you are performing any command in Render mode (Default graphics mode), you can hold down the middle mouse button to rotate the model.
What Delete the top portion of each rib. How Step
UI
Command/Display
1.
Delete, Geometry, Surface Menu
2.
Entity Selection dialog box: Pick the new surfaces that have been created on the top of each rib (see D in the following figure). OK OK
D
Notice: The top of each rib has been deleted.
14-8
Analyzing a Midsurface Model of an Electrical Box
What .Intersect the new ribs with the walls of the electric box.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Intersect Menu
2.
Entity Selection dialog box: Select All OK
Meshing the Model The first step in meshing the model is to assign mesh attributes for the different surfaces. If the correct attributes are not assigned, the results won’t be correct. Next, set the size for the mesh. Finally, mesh the midsurface.
Assigning Mesh Attributes What Assign the mesh attributes to the surfaces.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Assign Mesh Attributes Menu
2.
Entity Selection dialog box: Select All OK
3.
Define Material - ISOTROPIC dialog box: Load Pick a AISI 4340 Steel. OK (all dialog boxes)
Meshing the Model
Step
UI
14-9
Command/Display Tip: If midsurfaces are created manually using commands such as Geometry, Surface, Offset or Geometry, Surface, Extrude, the surfaces do not have mesh attributes. You must manually assign mesh attributes by creating or assigning existing properties using the correct thickness.
Meshing the Model What Set the mesh size to the default value, and mesh the model.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
2.
Entity Selection dialog box: Select All OK (all dialog boxes), then... Cancel
3.
Mesh, Geometry, Surface Menu
4.
Entity Selection dialog box: Select All OK
5.
Automesh Surfaces dialog box: Quads OK
14-10 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
Applying Loads and Constraints To load the model, you will apply a pressure to the surface at the back of the part. You will also constrain the holes at the base.
What Create a load set, the apply a pressure to the back of the part.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set OK 2.
Model, Load, On Surface Menu
3.
Entity Selection dialog box: ID: 185 OK Notice: Surface 185 is the middle surface at the back of the part.
4.
Create Loads on Surfaces dialog box: Pressure
5.
Pressure: Value: -1 OK
Applying Loads and Constraints
Step
UI
14-11
Command/Display
V1 L1 1.1. 1. 1. 1. 1.1. 1. 1. YZ X What Constrain the holes at the bottom of the part.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set OK 2.
Model, Constraint, On Curve Menu
3.
Entity Selection dialog box: Pick the eight curves around the holes at the base. OK Tip: You may want to rotate the model and zoom in on the corners of the model to make selection of these curves easier. While in a command you can use the middle mouse button to rotate the model as well as the Zoom and Previous Zoom icons on the View Toolbar.
4.
Create Constraints on Geometry dialog box: Pinned - No Translation OK
14-12 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
V1 L1 C1 TT TT Y ZX Tip: To see the nodes on which the loads and constraints are applied, use the Model, Load, Expand and Model, Constraint, Expand commands.
Analyzing the Model Solve the model using the NX Nastran solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Create an analysis set.
2
Analysis Program: 36..NX Nastran Analysis Type: 1..Static OK
3.
Analyze
Post-processing the Results For this analysis, you will display deformation and stress contours.
What Display and deformed/contour plot of translation and stress.
Post-processing the Results
14-13
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Deformation: 1..Total Translation Output Vectors: Contour: 7026..Plate Top MajorPrn Stress OK (all dialog boxes)
5. 6.
Ctrl-Q
View Quick Options Geometry Off UNCHECK Node in the Mesh Section Done
7.
Rotate the model so that you can see the back.
Notice: You can see the plate top stress contour on both faces of the plate elements.
14-14 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
What Change the contour options to display double-sided planar contours. If you select a standard top or bottom plate vector for contouring, as you did above, FEMAP can automatically contour both top and bottom stresses on the same plot. How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Select PostProcessing Data dialog box: Contour Options
4.
Select Contour Options dialog box: Contour Type: Elemental
5.
Data Conversion: Average
6.
Data Conversion: Use Corner Data
Post-processing the Results
Step 7.
UI
14-15
Command/Display Other Options: Double-Sided Planar Contours OK (all dialog boxes) Notice: The display has changed. The contour now shows plate top major principle stress on the top face of the plate elements and plate bottom major principle stress on the bottom face of the plate elements.
8.
Rotate the model to look at the back.
Notice: The contour on the back of the part shows plate top major stress.
14-16 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
What To more easily see double-sided results, change the view to show the element thicknesses.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Options: Element - Orientation/Shape, then... Element Shape: Show Fiber Thickness Tip: You can also “toggle” the thickness of planar elements on/off using the “Thickness/ Cross Section” command from the View Style menu located on the View Toolbar.
3.
Tools and View Style
4.
Filled Edges
5.
UNCHECK Draw Entity OK
Post-processing the Results
Step
UI
14-17
Command/Display Tip: You can also toggle the “Filled Edges” on and off very easily using the View Style menu located on the View Toolbar. Simply select Filled Edges from the View Style menu to turn them off, then select the command again to turn them back on at any time. Notice: The stress is now shown through the element thickness.
This is the end of the example. You don’t need to save your model file.
14-18
Analyzing a Midsurface Model of an Electrical Box
Direct Transient Analysis – Hinge Model 15.
Dynamic Analysis is used when a structure undergoes loading that occurs over time as opposed to static analysis which only takes into account the behavior of a structure at one time step. In many ways dynamic analysis is a more realistic type of analysis as compared to static analysis, but is also more complex. The loading is applied as a function of time during dynamic analysis, therefore, responses to the loading such as displacements, velocities, accelerations, forces, and stresses are also time-varying. For our first exploration of dynamic analysis, we will look at Direct Transient Analysis. Direct Transient Response can be used to determine a structure’s response to a time-varying excitation where all of the applied forces are known for each instant of time. In many cases, the desired responses to be computed are nodal displacements and accelerations, as well as, element forces and stresses.
Hinge Bracket
For this example we will be using a model of a hinge bracket that has already been created. You will work through the entire analysis process which includes:
· creating a loading function to represent sinusoidal excitation
· applying loads and constraints
· analyzing the model using NX Nastran
· post-processing the results using XY plotting capabilities
15-2
Direct Transient Analysis – Hinge Model
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/hinge.neu Locate hinge.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Creating the Dynamic Loading Function
Importing the Model
15-3
In order for the loading to be time dependent we must create a function to represent a sine pulse loading condition.
What Create a function to be used for applying a dynamic load How
Step 1.
UI
Command/Display Model, Function
Menu
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu).
2.
In Function Definition dialog box:
3.
Type “200 Hz sinusoidal pulse” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Equation radio button
15-4 5.
Direct Transient Analysis – Hinge Model
Enter the following values in the corresponding fields:
X = 0.0 To X = 0.005 Delta X = (0.005/8) Y = sin(360*200*!x)
Notice: The equation used in the Y field uses a formula creation syntax that FEMAP can read. For example the “sin” portion of the equation is telling FEMAP to take the sine of the value that is in the parenthesis (). The “!x” represents the variable x value as x increases from 0.0 to 0.005 based on the Delta X value (0.005/8 = 0.000625 for this example which will give us the needed 8 data points for our sine wave). The “200” value is our frequency in Hz. Click More button
6.
X and Y Values will be created for the function.
We need to “Zero” the curve after one single pulse, therefore we need to add one point with a “zero” Y value and a X value larger than 0.005
7.
Notice: NX/NASTRAN will use the curve coordinates for interpolation purposes and this is why the “zero” point must be added. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X =.0055 Click OK, then…
Y = 0.00
Click Cancel What Verify the function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Importing the Model
15-5
2.
In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..200 Hz sinusoidal Pulse” from Select drop down menu located in the Function portion of the window Click OK button
In View Select dialog box:
Click OK button Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key) The XY Plot should show a sine wave which levels off at the right hand side as shown below.
15-6
Direct Transient Analysis – Hinge Model
Creating the Transient Load What Apply the transient load to the hinge bracket
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose the Draw Model radio button Click OK
4.
The model should be on the screen again at this point. Model, Load, Set Menu
5.
In Create or Activate Load Set dialog box:
6.
Type “Transient Load” in the Title field Click OK
7.
Model, Load, Nodal Menu
8.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 44 at bottom right of structure
from the View Toolbar
Defining the Transient Analysis Parameters
15-7
Node 44
9.
Click OK
10.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 11.
Enter “75” into the FZ field
12.
Select “1..200 Hz Sinusoidal Pulse” from the Time/Freq Dependence drop down menu
13.
Click OK, then…
Click Cancel
Defining the Transient Analysis Parameters In order for NX Nastran to perform a direct transient analysis, there are certain parameters which must be defined within the Load Set. This will allow NX Nastran to know the number of desired time steps (each time step will produce an individual results set), the output interval, as well as, take into account the effects of damping. What Define the Dynamic Analysis Parameters
How
Step 1.
UI Menu
Command/Display Model, Load, Dynamic Analysis
15-8
Direct Transient Analysis – Hinge Model
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Direct Transient radio button Enter the following values in the corresponding fields:
Overall Structural Damping Coefficient (G) = 0.2 Frequency for System Damping (W3) = 90 Number of Steps = 99 (100 results sets produced including t=0) Time per Step = 0.0005 Output Interval = 1
4.
Notice: The Overall Structural Damping Coefficient (G =2 * (critical damping ratio)), therefore the system will experience 10% equivalent viscous damping. The Frequency for System Damping value of 90 was chosen because it is the first fundamental bending mode of this structure (This value is obtained from a normal modes analysis). The output interval of 1 will create an output set in the results file for every time step that is calculated, a value of 2 would create an output set for every other time step that NX Nastran calculates, and 3 would be every third time step and so on. Click OK
Creating the Constraints The model needs to be constrained for this example
What Create a constraint set and apply fixed nodal constraints
Defining the Transient Analysis Parameters
15-9
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Hole fixed” in the Title field Click OK button
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the nodes around the edge of the hole. This can be done by selecting one node at a time or… by holding down the Control (Ctrl) key and clicking near the center of the circle and dragging the mouse out which will create a circular picking window. Once all of the nodes are inside the circular picking window let go of the mouse button and all the nodes will be selected.
Notice: Holding down the Shift Key can also create a rectangular picking area and other picking options such as polygon, freehand, and query are available by pressing the “Pick” button inside any Entity Selection dialog box.
Nodes to be constrained
15-10 6.
Direct Transient Analysis – Hinge Model
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed Button, then…
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Setting up the Analysis Set Manager It is possible to save multiple Analysis Sets or “Cases” along with your FEMAP model. This will enable you to create multiple Analysis Cases and then select the appropriate case to be submitted to NX Nastran. For example, you can set-up one case to perform a Static analysis, one for Modal Analysis, another for Direct Transient Analysis, and yet another for Heat Transfer. All the cases can be saved with one model along with the different boundary conditions required for each separate analysis in separate load and constraint sets. You can also submit jobs to NX Nastran directly from the case manager by pressing the Analyze button.
What Create an analysis case for Direct Transient Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
Setting up the Analysis Set Manager
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Direct Transient Case” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
15-11
Select “3..Transient Dynamic/Time History” from the Analysis Type drop down menu
5.
Click OK
15-12
Direct Transient Analysis – Hinge Model
Advanced Nastran Notice: There are many NX Nastran options that can be selected and then saved using the Analysis Set Manager. These options include NASTRAN Executive and Solution controls, Bulk Data options, Element Quality Checks, Overall Model Checks, Specific Analysis Type Options, selection of Boundary Condition sets, Output Requests, and many others. The dialog boxes for each “group” of options can be reached by pressing the Next button on the Analysis Set dialog box, selecting the desired options in that specific dialog box, and then pressing the Next button again to progress to the next group of options.
For this particular example we will be using the defaults, so it is not required to alter these options to perform this analysis. Advanced Nastran Notice: For users familiar with any Nastran solver who would like to visually inspect the input deck before it is sent to the solver this can be accomplished by clicking the Preview Input button in the Analysis Set Manager dialog box. This will bring up a text viewer containing the Nastran input deck, and the viewer can become an editor by checking the box under Edit Preview. In Analysis Set Manager dialog box:
6.
Click Analyze button The Analysis should now be running, when it is complete results will be available for post-processing.
Post-Processing the Results In many cases, the results of Dynamic Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the response of a single node across the entire time history of the analysis. For this example we will use the loaded node, node number 44.
What Create a XY Plot of response of a single node of the structure
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
on the View Toolbar
Post-Processing the Results
4.
15-13
In Select XY Curve Data dialog box:
Select “1..Case 1 Time 0.” from drop down menu located in the Output Set section, then…
5.
Select “4..T3 Translation” from drop down menu located in the Output Vector section Enter “44” in the Node field located in the Output Location section
6.
In the Show Output Sets section, leave the From and To fields blank (By leaving these fields blank, the results at all output sets will be shown) Click OK, then…
In View Select dialog box:
Click OK The XY Plot the Z-translation of Node 44 should appear like this:
The XY Plot can be manipulated to take a closer look at a certain portion of the plotted response. The largest deflections of the loaded Node 44 occur between 0 and 0.03 on the X-Axis (Time), therefore we will change the range of the X-axis in order to zoom in on this part of the plot.
15-14
Direct Transient Analysis – Hinge Model
What Change the range of the X-axis on the XY Plot of Node 44
How
Step 1.
UI
Command/Display View, Options or…
Menu
2.
3.
4.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
Choose PostProcessing radio button under Category Highlight “XY X Range/Grid” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Max Min” from the Axis Range selection list Enter the following Values in the corresponding fields: Minimum = 0.0 Maximum = 0.03
5.
on the View Toolbar
Click OK
Post-Processing the Results
15-15
The Plot should now appear like this:
This Concludes the Direct Transient Analysis example. It is your choice whether or not to save the model file.
15-16
Direct Transient Analysis – Hinge Model
Modal Frequency Analysis of the Hinge Model 16.
Modal Frequency Response Analysis is used to determine a structure’s response to harmonic (oscillatory) excitation where all forces at each forcing frequency are known and defined within a frequency domain. The responses consist of complex numbers defined as magnitude and phase or as real and imaginary components.
First a Normal Modes Analysis will be run on the Hinge model to determine the natural frequencies. By using an NX Nastran option which allows analysis restarts, we will then perform a modal frequency response analysis without extracting the normal modes again. The purpose of this example is to determine the hinge structure’s response to a loading of unit amplitude across a frequency range up to 600 Hz. This frequency range has been chosen based on a prior normal modes analysis and contains the first three modes of the structure. We will assume the critical damping of the system to be 10%.
For this example we will be using a model of a hinge bracket that has already been created. You will work through the entire analysis process which includes:
· utilizing analysis restarts in NX Nastran to increase solution efficiency
· creating functions to define unit amplitude for frequency response loading and modal damping table
· analyzing the model using NX Nastran Frequency/Harmonic Response solution
· post-processing the results data using XY plotting capabilities
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI Menu
Command/Display File, New
16-2 2.
Modal Frequency Analysis of the Hinge Model
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/hinge.neu Locate hinge.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Creating the Constraints The model needs to be constrained for this example
What Create a constraint set and apply fixed nodal constraints
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Running the Normal Modes Analysis
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Hole fixed” in the Title field Click OK
4.
16-3
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples.
Nodes to be constrained
6.
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
Running the Normal Modes Analysis
16-4
Modal Frequency Analysis of the Hinge Model
Extracting the normal modes will enable NX Nastran to select solution frequencies automatically in order to create a solution frequency function. We will also take advantage of the analysis restarts option to transition from normal modes analysis to frequency response analysis.
What Create an analysis case for Normal Analysis and specify analysis restarts using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Normal Modes Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “2..Normal Modes/Eigenvalue” from the Analysis Type drop down menu
5.
Click Next
6.
In NASTRAN Executive and Solution Options dialog box:
CHECK Save Databases for Restart box in the Restart Control section
Notice: Make sure the files that NX Nastran will be using for the Restart are in a directory where none of the directory names has a space in it. For Example: If the path to the *.MASTER would be C:\Analysis Files\filename.MASTER, NX Nastran will not be able to get to the restart file. A path such as C:\Analysis_Files\filemane.MASTER would be able to be run because the directory name has an underscore instead of a space.
Creating Unit Load for Frequency Response Loading
7.
16-5
Click OK
In Analysis Set Manager dialog box:
Click Analyze button IMPORTANT: Once the Normal Modes Analysis has been completed, verify that results have been retrieved from NX Nastran by pressing the F5 key (View Select command) and then clicking the “Deformed and Contour Data” button. In the Select Post Processing dialog box under Output Set make sure “1.Mode 1, 89.81622 Hz” is visible (If there are no results, then the analysis may not have completed successfully and therefore the model should be checked for mistakes and then rerun). Click OK and OK again.
Also be sure that the NX Nastran databases (the *.MASTER and *.DBALL files, “*”denotes the filename the user has given to this example when saved before running the analysis) have been saved for “Restart” purposes in the directory where the analysis has taken place (should be in the same directory as where the results files, *.op2 and *.f06, can be found).
Creating Unit Load for Frequency Response Loading A Unit Load must be created to remain constant across the entire frequency range. A simple function will be used to represent the temporal portion of the load and then given a direction to represent the spatial portion of the loading condition.
What Create a function for the Unit Load
16-6
Modal Frequency Analysis of the Hinge Model
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Load Value vs. Frequency” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 1, Then…Click More button X = 1, Y = 1 Click OK, then...
6.
Click Cancel
What Apply the 1.0 unit load to the hinge bracket
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
Type “Unit Load” in the Title field
Creating Unit Load for Frequency Response Loading
3.
16-7
Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 44 at bottom right of structure
Node 44
6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “1.0” into the FZ field
9.
Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
10.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel The Frequency Response Loading Condition has now been applied.
Modal Damping Definition
16-8
Modal Frequency Analysis of the Hinge Model
A simple function must be created to represent the modal damping of the system. The type of function created depends on the units of the assumed damping value:
1. If the structural damping coefficient (G) is known, then Function Type “6..Structural Damping vs. Freq” should be used.
2. If the critical damping ratio is known, then Function Type “7..Critical Damping vs. Freq” should be used.
3. If the Quality/Magnification Factor (Q) is known, then Function Type “8..Q Damping vs. Frequency” should be used.
In our case, a critical damping ratio of 10% across the frequency range is desired. Therefore, we will use the Function Type “7..Critical Damping vs. Freq”. What Create a function to represent the desired Critical Damping for the system.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Damping Function” in the Title field Select “7..Critical Damping vs. Freq” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0.1, Then…Click More button
6.
X = 1, Y = 0.1 Click OK, then...
Click Cancel
Defining Solution Frequencies
Creating Unit Load for Frequency Response Loading
16-9
Solution Frequencies can be defined two separate ways. One way is to create a function which gradually raises the frequency in defined increments in a given frequency range. If you have not extracted the normal modes in a previous analysis, this is a way to create a frequency table to excite the structure. The disadvantage of this method is that it will give you a large number of data points to review in general and not concentrate the results around the natural modes, where the response should be the highest.
Because we have run a normal modes analysis, and NX NASTRAN has the Analysis Restart capability we set-up earlier, we can use a different and more effective method to create our frequency table. Utilizing the known results of the normal modes analysis we ran earlier in the tutorial, FEMAP can create a much more accurate frequency table for Modal Frequency Response. The frequency table, along with other parameters, must be defined within the Load Set before the Hinge model can be analyzed.
What Define the Frequency Table and Modal Frequency Response parameters
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Modal Frequency radio button Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section
4.
Click Modal Freq...button
5.
In Frequency Table From Modal Results dialog box:
Select “1..Mode 1, 89.81622 Hz” from the First Freq drop down menu, then…
6.
Select “3..Mode 3, 568.1597 Hz” from the Last Freq drop down menu Enter the following values into the corresponding fields:
Number of Point per Existing Modes = 5 Frequency Band Spread = 10 (%)
Notice: These values, 5 per Existing Mode and 10% Frequency Band Spread, are somewhat standard for creating the Frequency Table using existing Normal Modes.
16-10
7.
Modal Frequency Analysis of the Hinge Model
Click OK
In Load Set Options for Dynamic Analysis dialog box:
8.
Make sure “3..Modal Frequency Table” appears in the Frequencies drop down menu in the Frequency Response section. Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
Notice: The Overall Structural Damping Coefficient (G) does not need to be defined because we have already taken care of this with the function created for the Modal Damping Table.
Creating Unit Load for Frequency Response Loading
9.
16-11
Click OK
Visual verification of the Frequency Table function in a XY Plot is always a good check before analyzing the model.
What Verify the Frequency Table function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “3..Modal Frequency Table” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key)
16-12
Modal Frequency Analysis of the Hinge Model
The XY Plot should show three peaks, one peak for each of the first three modes. The Y value is arbitrary on this plot, but the x-values are an excellent way to visualize where the excitations are occurring with respect to the frequency range. Also, the width of the base of each peak represents the frequency bandwidth associated with each forcing frequency.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Modal Frequency Response Analysis What Create an analysis case for Modal Frequency Response Analysis and specify analysis restarts using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
Enter “Modal Frequency Response Analysis” in the Title field
Running the Modal Frequency Response Analysis
4.
16-13
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
5.
Click Next
6.
In NASTRAN Executive and Solution Options dialog box:
7.
CHECK Restart Previous Analysis box in the Restart Control section Click the Browse button (“...” button) and locate the “*.MASTER” file that was created earlier in the tutorial. Remember, this should be located in the same directory as your Normal Modes Analysis Results File. Then…
Click Open
16-14 8.
Modal Frequency Analysis of the Hinge Model
Click OK
In Analysis Set Manager dialog box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the response of a single node across the entire frequency range of the analysis. For this example we will use the loaded node, node number 44.
What Create a XY Plot of response of a single node of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
from the View Toolbar
Select “11..Case 1 Freq 80.83459” from drop down menu located in the Output Set section, then…
5.
Select “4..T3 Translation” from drop down menu located in the Output Vector section Enter “44” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “25” in the To field in the Show Output Sets section
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the frequency response of Node 44.
Post-Processing the Results
6.
16-15
Click OK, then…
In View Select dialog box:
Click OK The resulting XY Plot will show the Z-Translation of Node 44 across the entire frequency range.
This concludes the Modal Frequency Response Analysis example. Please save this model as Hingemodal.mod for use in a later tutorial.
16-16
Modal Frequency Analysis of the Hinge Model
Frequency Response of Tower with Seismic Excitation 17.
This example will move step by step through a Frequency Response Analysis of a tower being forced at a base node with a 1g sinusoidal (Seismic) loading condition. The model of the tower has been constructed and a modal analysis has been run previously. We will import the model and concentrate on the creation of Frequency Response loading conditions, the two different methods of applying the excitation to the model (Large Mass and Direct Methods), and post-processing the results of the analysis by examining accelerations of specific nodes.
Large Mass Method
Direct Method
For this example we will be using a model of a communications tower that has already been created. You will work through the entire analysis process which includes:
· creating a loading condition to represent a seismic excitation
· applying loads and constraints specific to both methods of creating the excitation
· analyzing the model using NX Nastran
· post-processing the results using multiple curves in XY plots.
17-2
Frequency Response of Tower with Seismic Excitation
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/tower.neu Locate tower.neu
Click Open
Neutral File Read Options dialog box:
Click OK
View the results of Modal Analysis
Importing the Model
17-3
What View an animation of the Mode Shapes created by the Natural Frequencies
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate radio button in the Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Mode 1, 10.8234 Hz” from the drop down menu in the Output Set section
Select “1..Total Translation” from Deformation drop down menu in the Output Vector section Click OK
5.
In View Select dialog box:
Click OK
The Model should now be moving based on the first Natural Frequency.
What Change the Output Set (Mode Shape) being viewed a few different ways
How You can follow Steps 1-3 above, then Select “The mode you want to view” from the drop down menu in the Output Set section, then follow Steps 5-6.
OR
Step
UI
Command/Display
17-4
Frequency Response of Tower with Seismic Excitation
1.
Click the Right Mouse button and highlight Post Data
2.
In Select PostProcessing Data dialog box:
3.
Select “The mode you want to view” from the drop down menu in the Output Set section Click OK
OR
Step 1.
UI Menu
Command/Display Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) This will bring up the Post Toolbar.
Click the Next Set icon or the Previous Set icon to move back and forth through the existing Output Sets (These icons are located on the Post Toolbar)
Notice: The Toolbars contain many popular commands that can be accessed in one click or choosing off a short menu instead of through multiple cascading menus and/or dialog boxes. Take some time to become familiar with some of the features conveniently located on the Command Toolbar.
After all of the Mode Shapes have been viewed:
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose None-Model Only radio button in the Deformed Style section Click OK
Modal Damping Definition
from the View Toolbar
Creating Function for Seismic Loading
17-5
A simple function must be created to represent the modal damping of the system. The type of function created depends on the units of the assumed damping value:
What Create a function to represent the desired Critical Damping for the system.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Damping Function” in the Title field Select “7..Critical Damping vs. Freq” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0.1, Then…Click More button
6.
X = 1, Y = 0.1 Click OK, then...
Click Cancel
Creating Function for Seismic Loading A Function must be created to remain constant across the entire frequency range. A simple function will be used to represent the temporal portion of the load and then given a direction and magnitude to represent the spatial portion of the loading condition later in the example
What
17-6
Frequency Response of Tower with Seismic Excitation
Create a function for the Seismic Loading
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “1g Loading” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 1, Then…Click More button
X = 1, Y = 1 Click OK, then...
6.
Click Cancel
Defining Solution Frequencies
As in our Modal Frequency Example 16 we will create our Solution Frequency Table using our existing Modal Analysis.
What Define the Frequency Table and Modal Frequency Response parameters
How
Step 1.
UI Menu
Command/Display Model, Load, Set
Creating Function for Seismic Loading
2.
In Create or Activate Load Set dialog box:
3.
Type “Seismic Load” in the Title field Click OK
4.
17-7
Model, Load, Dynamic Analysis Menu
5.
In Load Set Options for Dynamic Analysis dialog box:
6.
Choose Modal Frequency radio button Select “1..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section
7.
Click Modal Freq...button
8.
In Frequency Table From Modal Results dialog box:
Select “1..Mode 1, 10.8234 Hz” from the First Freq drop down menu, then…
9.
Select “5..Mode 5, 28.03074 Hz” from the Last Freq drop down menu Enter the following values into the corresponding fields:
Number of Point per Existing Modes = 5 Frequency Band Spread = 10 (%)
Notice: These values, 5 per Existing Mode and 10% Frequency Band Spread, are somewhat standard for creating the Frequency Table using existing Normal Modes.
17-8 10.
Frequency Response of Tower with Seismic Excitation
Click OK
In Load Set Options for Dynamic Analysis dialog box:
Make sure “3..Modal Frequency Table” appears in the Frequencies drop down menu in the Frequency Response section. Enter the following values in the corresponding fields:
11.
Highest Freq (Hz) = 200
Notice: The Overall Structural Damping Coefficient (G) does not need to be defined because we have already taken care of this with the function created for the Modal Damping Table. Click OK
12.
Creating the Base Node and Rigid Connection What Create the Base Node (Node which will have excitation applied)
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Enter the following values into the corresponding fields:
3.
X = 0, Y = -220, Z = 0 Click OK, then…
Click Cancel
What Create Rigid Connection between Base Node and Tower
How
Creating the Base Node and Rigid Connection
Step 1.
UI
17-9
Command/Display Model, Element
Menu
2.
In the Define PLATE (or “Type of Element”) Element – Enter Nodes or Select with Curser dialog box:
3.
Click Type button In the Element/Property Type dialog box:
4.
Choose Rigid radio button in the Other Elements section Click OK
5.
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
6.
Choose the newly created node located below the tower (node 269) for the node in the Independent section UNCHECK the RX, RY, and RZ boxes in the Independent section
7.
Click Nodes button in the Dependent portion of the dialog box
8.
In the Entity Selection – Select Master Node(s) dialog box:
Select the node at the bottom of each “leg” of the tower (nodes 50, 61, 67, and 78)
Nodes to be selected 9.
Click OK
17-10
10.
Frequency Response of Tower with Seismic Excitation
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
Click OK, then…
Click Cancel IMPORTANT: At this point the exercise will have two separate sections. One section will cover the “Large Mass Method” and the other will cover the “Direct Method” of creating a seismic loading condition. Please give both methods a try. Save your model at this point as tower.mod, in order to have a good starting point for the two separate sections.
Large Mass Method Creating the Seismic Mass
What Create Mass Property and then Mass Element
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In the Define Property – RIGID (or “Type of Element”) Element Type dialog box:
3.
Click Elem/Property Type button In the Element/Property Type dialog box:
4.
Choose Mass radio button in the Other Elements section Click OK
Large Mass Method
5.
In the Define Property – MASS Element Type dialog box:
Type “Base Mass” in the Title field
Enter “1.0E13” in the Mass, M or Mx field
6.
Click OK, then…
7.
Click Cancel Model, Element Menu
8.
In Define MASS Element – Enter Node or Select with Cursor dialog box:
Select the Base Node (Node 269) 9.
Select “3..Base Mass” from the Property drop down menu
10.
Click OK, then…
Cancel Creating the Load and Permanent Constraints
What Create Load for Large Mass
17-11
17-12
Frequency Response of Tower with Seismic Excitation
How
Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Base Node (node 269) 3.
Click OK
4.
In the Create Loads on Nodes dialog box:
Highlight Force from the selection list 5.
Enter “386.4E13” into the FX field
6.
UNCHECK the FY and FZ boxes
7.
Select “2..1g Loading” from the Time/Freq Dependence drop down menu
8.
Click OK, then…
Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
What Create Permanent Constraints on the Base Node
How
Step 1.
UI
Command/Display Modify, Edit, Node
Menu
2.
Entity Selection – Select Node(s) to Edit dialog box:
Select the Base Node (node 269)
Running the Seismic Analysis
3.
17-13
Click OK, then…
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click Parameters button In the Node Parameters dialog box:
4.
CHECK the TY, TZ, RX, RY, and RZ boxes in the Permanent Constraint section
Notice: This will create Permanent Constraints on the Node Entry in the NX NASTRAN input file (GRID,269,0,0.,-220.,0.,0,23456). These type of constraints do not require a defined constraint set, NX NASTRAN understands that this particular node is constrained in the 23456 degrees of freedom for any analysis regardless of other Constraint Sets. Click OK, then…
5.
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click OK THE MODEL IS NOW READY TO BE ANALYZED!
Running the Seismic Analysis What Create an analysis case for Seismic Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager Dialog Box:
3.
Click New button In Analysis Set Dialog Box
Type “Seismic Analysis” in the Title field
17-14 4.
Frequency Response of Tower with Seismic Excitation
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
5.
Click OK
In Analysis Set Manager Dialog Box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the nodal accelerations of a few nodes across the entire frequency range of the analysis. For this example we will use the view the accelerations at node numbers 75, 249, and 151.
What Create a XY Plot of the responses of multiple nodes of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
from the View Toolbar
Post-Processing the Results
4.
17-15
In Select XY Curve Data dialog box:
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
5.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “75” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
6.
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the accelerations. Choose “2” radio button in the Curve section
7.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
8.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “249” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
9.
Enter “35” in the To field in the Show Output Sets section Choose “3” radio button in the Curve section
10.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
11.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “151” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
12.
Enter “35” in the To field in the Show Output Sets section Click OK, then…
In View Select dialog box:
Click OK
17-16
Frequency Response of Tower with Seismic Excitation
The XY Plot of the accelerations at nodes 75, 249, 151 should look like this:
This concludes the Seismic Analysis using the Large Mass Method section of the example. Please save this model as TowerLMM.mod. Please open the Tower.mod model that you saved earlier in the example and we will now complete the analysis using the Direct Method.
Direct Method Creating the Load and Permanent Constraints
What Create Acceleration Load
How
Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Base Node (node 269) 3.
Click OK
Direct Method
4.
In the Create Loads on Nodes dialog box:
Highlight Acceleration from the selection list 5.
Enter “386.4” into the AX field
6.
UNCHECK the AY and AZ boxes
7.
Select “2..1g Loading” from the Time/Freq Dependence drop down menu
8.
Click OK, then…
Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Create constraints on the Base Node
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed Base Node” in the Title field Click OK button
4.
Model, Constraint, Nodal Menu
5.
In Entity Selection – Enter Node(s) to Select dialog box
Select the Base Node (Node 269)
17-17
17-18 6.
Frequency Response of Tower with Seismic Excitation
Click OK, then...
In Create Nodal Constraints/DOF dialog box:
Click the Fixed Button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Seismic Analysis What Create an analysis case for Seismic Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Seismic Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
Post-Processing the Results
5.
Click Next button 2 times, then…
6.
In NASTRAN Bulk Data Options dialog box:
17-19
CHECK the box next to RESVEC (make sure it also is set to “On”)
Notice: It is highly recommended during Frequency Response where the Direct Method is used that the Residual Vector Parameter (RESVEC) be used for increased solution accuracy. Click OK, then…
7.
In Analysis Set Manager dialog box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the nodal accelerations of a few nodes across the entire frequency range of the analysis. For this example we will use the view the accelerations at node numbers 75, 249, and 151.
What Create a XY Plot of the responses of multiple nodes of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
17-20
Frequency Response of Tower with Seismic Excitation
2.
In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
5.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “75” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
6.
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the accelerations. Choose “2” radio button in the curve section
7.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
8.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “249” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
9.
Enter “35” in the To field in the Show Output Sets section Choose “3” radio button in the curve section
10.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
11.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “151” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
Post-Processing the Results
12.
Click OK, then…
In View Select dialog box:
Click OK The XY Plot of the accelerations at nodes 75, 249, 151 should look like this:
This concludes the Seismic Analysis example. Please save this model as TowerDM.mod.
17-21
17-22
Frequency Response of Tower with Seismic Excitation
Random Response of the Hinge Model 18.
Random Frequency (Vibration) Response can be used to simulate such effects as earthquake ground motion, pressure fluctuations caused by wind on tall buildings and aircraft, and acoustic excitation due to jet and rocket engine noise. In NX Nastran, Random Response Analysis is performed as a “post-processing” to a previously completed Frequency Response Analysis. Random Response requires many of the same inputs used in Frequency Response, but also requires an additional user-defined loading condition such as a load governed by a Power Spectral Density (PSD) function.
There are two separate methods to create enforced base motion to excite the structure using NX Nastran. The first method is the “Large Mass method” which requires a load, such as a force, be applied to a “large mass” attached to the structure, which in this case will simulate an acceleration load. A Large Mass is described as an object (usually a single point mass) between 105 and 1013 times the mass of the structure. The other method is quite a bit easier to set-up and allows the user to apply the nodal load directly to a specific node and does not require the user to create a Large Mass in order to apply enforced motion. This “Direct Method” was developed for MSC.NASTRAN version 2001 and later (This includes all version of NX Nastran), therefore it should be the preferred method for those users who are learning to perform analyses involving enforced motion. We will explore both methods in this exercise. A great resource for Random Vibration Analysis is located at: http:// analyst.gsfc.nasa.gov/FEMCI/random/
For this example, you will need to have completed the Modal Frequency Response exercise to continue because we will be using the hingemodal.mod file you have saved. You will work through the entire analysis process which includes:
· creating a Power Spectral Density (PSD) function
· creating an enforced motion loading condition using the “Large Mass Method” and the “Direct Method”
· setting up a group in order to make specific output requests
· analyzing the model using NX Nastran Random Response solution
· post-processing results functions using XY plotting capabilities
Opening an Existing FEMAP Model What Open an existing FEMAP model file hingemodal.mod.
18-2
Random Response of the Hinge Model
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Dynamics/Random Response/hingemodal.mod
Click Open
Deleting existing Loads and Boundary Conditions
What Delete Load Sets and Constraint Sets.
How
Step 1.
UI Menu
Command/Display Delete, Model, Load Set
Defining the Power Spectral Density Function
2.
18-3
In Entity Selection – Select Load Set(s) to Delete dialog box:
Click Select All button, then…
Click OK, then…
In Confirm Delete dialog box:
Click OK Delete, Model, Constraint Set
3. Menu
4.
In Entity Selection – Select Constraint Set(s) to Delete dialog box:
Click Select All button, then…
Click OK, then…
In Confirm Delete dialog box:
Click OK Tip: You can quickly delete both Load and Constraint sets from the Model Info tree. Simply highlight either the “top-level” Loads branch or the Constraints branch, then right click and choose the Delete command form the “context sensitive menu” (this will delete ALL Load or Constraint sets). This command will also work with any individual Load or Constraint Sets.
Defining the Power Spectral Density Function Power Spectral Density (PSD) functions are created from empirical data recovered by accelerometers during dynamic testing (we will actually be creating an Acceleration Spectral Density (ASD) function which approximates the actual PSD plot, but will refer to it as a PSD function). For this example we are going to use a very basic PSD function in order to demonstrate the use of a PSD function in Random Response. The Units of our PSD function are G2/Hz, where G is Gravitational Acceleration vs. Frequency in Hz.
What Create a simple PSD function
How
Step
UI
Command/Display
18-4 1.
Random Response of the Hinge Model
Model, Function Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “PSD Function” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 20, Y = 0.1, Then…Click More button X = 40, Y = 1.0, Then…Click More button X = 100, Y = 1.0, Then…Click More button X = 350, Y = 0.1, Then…Click More button X = 700, Y = 0.1 Click OK, then...
6.
Click Cancel Visual verification of the PSD function in a XY Plot is always a good check before analyzing the model. What Verify the PSD function using the XY Plotting Feature of FEMAP How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
Choose XY of Function radio button
from the View Toolbar
Defining the Power Spectral Density Function
18-5
3.
Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “4..PSD Function” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK
Notice: In order to create an XY plot that is more representative of a PSD function we will want to view it in as a Log-Log Plot instead of the default Rectilinear format. View, Options or…
6. Menu
7.
8.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
Choose PostProcessing radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Log-Log” from the Plot Type selection list
9.
on the View Toolbar
Click OK
18-6
Random Response of the Hinge Model
The XY Plot should now look like this:
What Change View so model can be seen for selection purposes. How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Draw Model radio button Click OK
from the View Toolbar
IMPORTANT: At this point the exercise will split into two separate sections until it is time to analyze the model. One section will cover the “Large Mass Method” and the other will cover the “Direct Method” of Enforced Motion Application. If you are familiar with the “Large Mass Method” and plan to continue using this method, please continue on with the tutorial starting below this message. If you have not done Enforced Motion analysis before, we suggest you concentrate on the “Direct Method”, which starts on page (page 18-10), with the heading “Creating Enforced Motion Loading using the Direct Method”, because it is the updated means to perform an Enforced Motion Analysis. If you would like to give both methods a try, please save your model at this point as hingePSD.mod, in order to have a good starting point for the two separate sections.
Creating Enforced Motion Loading - Large Mass Method
18-7
Creating Enforced Motion Loading - Large Mass Method What Define the Random Frequency Response parameters and create Large Mass for Enforced Motion.
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
FEMAP will prompt you to Create a Load Set.
In Create or Activate Load Set dialog box:
3.
Type “Enforced Motion” in the Title field Click OK
4.
In Load Set Options for Dynamic Analysis dialog box:
5.
Choose Modal Frequency radio button Click Enforced Motion button
6.
FEMAP will ask for the coordinates of a “Base Mass”
In the Locate – Enter Coordinates for Base Mass dialog box:
Enter the following values in the corresponding fields:
X = -0.5, Y = 4, Z = 0 (This will position a point mass at the center of the hole)
7.
Click OK
18-8 8.
Random Response of the Hinge Model
Entity Selection – Select Nodes on Base dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples. A good idea here is holding the CTRL Key, selecting near the center of the hole and dragging the picking circle out until desired nodes are within circular picking area.
Nodes to be selected for base
9.
Click OK
10.
In the Create Loads on Nodes dialog box:
11.
Highlight Acceleration from the selection list if not already selected Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
12.
Check AZ box for text field to become available
13.
Enter “1.0” into the AZ field
Creating Enforced Motion Loading - Large Mass Method
14.
Click OK
15.
In Mass/Accel Scale Factor dialog box:
18-9
Verify the following fields:
Mass = 0.0070248, Factor = 1000000.
16.
Click OK
17.
In Load Set Options for Dynamic Analysis dialog box:
Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section, then…
Select “3..Modal Frequency Table” from the Frequencies drop down menu in the Frequency Response section, then…
Select “4..PSD Function” from the PSD drop down menu in the Random Analysis Options section
18-10 18.
Random Response of the Hinge Model
Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
19.
Click OK
Notice: A Mass Element with an acceleration load connected to the nodes around the hole with a Rigid Element has been created for Enforced Motion purposes.
Rigid Element
Mass Element
What Create a constraint set to constrain the excitation node in all directions except for the acceleration direction (Z-translation).
Creating Enforced Motion Loading - Large Mass Method
18-11
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
Type “1” in the ID field
Type “Load Constraint” in the Title field Click OK
3. 4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node “289” at the center of the circle 6.
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Fixed, then… 7. UNCHECK the TZ box (leaving the rest of degrees-of-freedom checked) 8.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel
IMPORTANT: You have finished creating the Enforced Motion portion of the Random Response Analysis tutorial using the “Large Mass” method. To learn how to analyze and post-process the results of the Random Response, please move ahead to the “Creating a Group for Output Request needs” portion of the tutorial. If you would like to try using the “Direct Method” to define Enforced Motion, save your model as hingeLMM.mod and open hingePSD.mod and continue with the tutorial below.
18-12
Random Response of the Hinge Model
Creating Enforced Motion Loading - Direct Method No Large Mass is required to apply an excitation such as acceleration to an individual node when the “Direct Method” is used to define Enforced Motion.
What Create a base node and connect it to the structure with a rigid element.
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Curser dialog box:
Enter the following values in the corresponding fields:
3.
X = -0.5, Y = 4, Z = 0 (This will position a node at the center of the hole) Click OK, then…
4.
Click Cancel Model, Element Menu
5.
In the Define PLATE (or “Type of Element”) Element – Enter Nodes or Select with Curser dialog box:
6.
Click Type button In the Element/Property Type dialog box:
7.
Choose Rigid radio button in the Other Elements section Click OK
8.
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
9.
Choose the newly created node at the center of the hole (node 289) for the node in the Independent section Click Nodes button in the Dependent portion of the dialog box
Creating Enforced Motion Loading - Direct Method
10.
18-13
Entity Selection – Select Master Node(s) dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples. A good idea here is holding the CTRL Key, selecting near the center of the hole and dragging the picking circle out until desired nodes are within circular picking area (this will pick the center node, but we will remove it from the selection list in the next step)
Nodes to be selected for base
11.
Highlight “+289” from the selection list if not already selected.
12.
Click Delete, then...
Click OK, then…
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
Click OK, then…
Click Cancel What Create an acceleration load directly on a node.
How
Step
UI
Command/Display
18-14 1.
Random Response of the Hinge Model
Model, Load, Set Menu
2.
In Create or Activate Load Set Dialog Box:
3.
Type “Acceleration Load” in the Title field Click OK button
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 289 at center of hole
Node 289
6.
Click OK
7.
In the Create Loads on Nodes dialog box
Highlight Acceleration from the selection list 8.
Enter “1.0” into the AZ field
9.
UNCHECK the AX and AY boxes
10.
Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
Setting the Random Response Parameters
11.
18-15
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel
Setting the Random Response Parameters What Define the parameters for Random Response Analysis
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Modal Frequency radio button Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section, then…
Select “3..Modal Frequency Table” from the Frequencies drop down menu in the Frequency Response section, then…
4.
Select “4..PSD Function” from the PSD drop down menu in the Random Analysis Options section Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
18-16
5.
Random Response of the Hinge Model
Click OK
Creating the Constraints The node being “excited” needs to be fixed (including in the direction of the acceleration) when using the Direct Method. This is a major difference between the Large Mass Method and the Direct Method.
What Create a constraint set and apply a “fixed” nodal constraint on the excited node.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Load Constraint” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
Creating a Group for Output Request needs
5.
18-17
Entity Selection – Enter Node(s) to Select dialog box
Select the node “289” at the center of the circle 6.
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Fixed, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel IMPORTANT: The tutorial is the same for both Enforced Motion Methods from this point except for one small difference which is documented in the “Running the Random Response Analysis” section.
Creating a Group for Output Request needs What Create a group containing a node in order to recover specific, requested output responses.
How
Step 1.
UI
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Results Nodes” in the Title field Click OK
4.
Group, Node, ID Menu
5.
In Entity Selection – Select Node(s) for Group dialog box:
Enter “44” into the ID field
18-18 6.
Random Response of the Hinge Model
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Random Response Analysis What Create an analysis case for Random Response Analysis and specify output requests using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Random Response” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “6..Random Response” from the Analysis Type drop down menu
5.
If you are using a previous version of NX Nastran for FEMAP (versions 8.3 to 9.1) and are using the “Direct Method” for this example, please read the notice below. There is a different process you will want to follow to get accurate results. If you used either method in NX Nastran for FEMAP version 9.2 or above, then simply... Click Next button 8 times
Running the Random Response Analysis
18-19
Notice: DO NOT DO THIS STEP IF YOU ARE USING THE LARGE MASS METHOD IN ANY VERSION OF NX NASTRAN FOR FEMAP OR THE DIRECT METHOD IN NX NASTRAN VERSION 9.2 OR HIGHER. It is not required for NX Nastran 4.1, which is in version of NX Nastran in FEMAP version 9.2. Click Next button 2 times, then in the NASTRAN Bulk Data Options dialog box, Check the box next to RESVEC, then…
Click Next button 6 times
6.
It is highly recommended during dynamic response analysis where enforced motion is employed using the Direct Method that the Residual Vector Parameter (RESVEC) be used for increased solution accuracy. In NASTRAN Output for Random Analysis dialog box:
CHECK both “T3” boxes for Displacement and Acceleration in the Nodal Output Request section (This will request XY data for the node across the frequency range)
7.
Click OK
8.
In Nodal Results dialog box:
Highlight “1..Results Nodes” from the Group selection list
18-20
Random Response of the Hinge Model
9.
Click OK
10.
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read PSD vs. Frequency Functions?”...Click Yes
Post-Processing the Random Response Analysis We have requested XY plotted data (PSD vs. Frequency functions) for the nodal acceleration and displacement for the node that we placed in our “Results Nodes” group. FEMAP will create functions representing this data. This data is available in the *.f06 print results file and NOT the *.op2 binary results file. Make sure to read in the *.f06 file in order to view the requested output.
What View the Acceleration results function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
from the View Toolbar
Select “6..ACC3 PSD Node 44” from Select drop down menu located in the Function portion of the window
Post-Processing the Random Response Analysis
5.
18-21
Click OK
In View Select dialog box:
Click OK View, Options or…
6. Menu
7.
8.
9.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “0..Rectilinear” from the Plot Type selection list Click OK
The plot of the Acceleration Function of Node 44 should look like this:
This completes the Random Response example. Save the model as hingerandom.mod.
18-22
Random Response of the Hinge Model
Generation of Response Spectra Single Degree of Freedom model 19.
Response Spectrum Analysis is used to approximate the peak response to a transient excitation at the base of the structure. It is a useful tool in determining the maximum response of a structure without regard to the exact time it is occurring. For instance, the effects an earthquake might have on a specific floor of a building or a smaller component on a ship being excited by an explosion. The results of the Response Spectrum can then be applied to a specific component to determine localized results such as stress. This type of analysis is also referred to as Shock Spectrum Analysis.
A very simple model will be created in order to demonstrate the techniques used in creating a Response Spectrum.
For this example a Single Degree-of-Freedom model will be used. You will work through the entire analysis process which includes:
· creating the Single Degree-of-Freedom model
· creating a loading function to represent sinusoidal excitation, as well as, functions to represent Oscillation Frequencies and Oscillation Damping
· analyzing the model using NX Nastran
· post-processing the acceleration of the nodal results using XY plotting capabilities
Creating the Model Our will have one node and one Unit Mass element. The node will be permanently constrained in all but the x-translation degree-of-freedom.
What Creating a Node with Permanent Constraints
How
Step
UI
Command/Display
19-2 1.
Generation of Response Spectra - Single Degree of Freedom model
File, New Menu
2.
Model, Node Menu
3.
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Enter the following values into the corresponding fields:
4.
X = 0, Y = 0, Z = 0 Click Parameters button
5.
In the Node Parameters dialog box:
6.
CHECK the TY, TZ, RX, RY, and RZ boxes in the Permanent Constraint section Click OK, then…
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click OK, then…
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Click Cancel What Create Mass Property and then Mass Element
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In the Define Property – PLATE (or “Type of Element”) Element Type dialog box:
Click Elem/Property Type button
Creating the Dynamic Loading Function
3.
In the Element/Property Type dialog box:
4.
Choose Mass radio button in the Other Elements section Click OK
5.
In the Define Property – MASS Element Type dialog box:
19-3
Type “Base” in the Title field
6.
Enter “1.0” in the Mass, M or Mx field Click OK, then…
7.
Click Cancel Model, Element Menu
8.
In Define MASS Element – Enter Node or Select with Cursor dialog box:
Select the Node 9.
Select “1..Base” from the Property drop down menu
10.
Click OK, then…
Cancel
Creating the Dynamic Loading Function In order for the loading to be time dependent we must create a function to represent a sine pulse loading condition.
What Create a function to be used for applying a dynamic load
How
Step 1.
UI Menu
Command/Display Model, Function
19-4
Generation of Response Spectra - Single Degree of Freedom model
2.
In Function Definition dialog box:
3.
Type “200 Hz sinusoidal pulse” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Equation radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 0.005 Delta X = (0.005/8) Y = sin(360*200*!x)
Notice: This is the same function that was created in the Direct Transient example. 6.
Click More button
X and Y Values will be created for the function. A “Zero” value must be given after one single pulse, therefore we need to add one point with a “zero” Y value and a X value larger than 0.005
7.
Notice: NX Nastran will use the curve coordinates for interpolation purposes and this is why the “zero” point must be added. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X = 0.0055 Click OK, then…
Y = 0.00
Click Cancel What Verify the function using the XY Plotting Feature of FEMAP
How
Step
UI
Command/Display
Creating the Load
1.
19-5
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..200 Hz sinusoidal Pulse” from Select drop down menu located in the Function portion of the window Click OK button
In View Select dialog box:
Click OK button The XY Plot should show a sine wave shown below.
Creating the Load What Create a nodal load
How
Step
UI
Command/Display
from the View Toolbar
19-6 1.
Generation of Response Spectra - Single Degree of Freedom model
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose the Draw Model radio button Click OK
4.
The model should be on the screen again at this point. Model, Load, Set
from the View Toolbar
Menu
5.
In Create or Activate Load Set dialog box:
6.
Type “Base Excitation” in the Title field Click OK
7.
Model, Load, Nodal Menu
8.
Entity Selection – Enter Node(s) to Select dialog box:
Select Node 1 9.
Click OK
10.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 11.
Enter “1.0” into the FX field
12.
UNCHECK the FY and FZ boxes
13.
Select “1..200 Hz Sinusoidal Pulse” from the Time/Freq Dependence drop down menu
14.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
Creating the Load
19-7
Creating the Oscillator Functions to Generate Response Spectra
Functions for the Frequency range and the Damping values must be created in order to generate the desired results from the analysis
What Create a function for the Response Spectrum Frequencies
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Oscillator Frequencies” in Title field Select “0..Dimensionless” from Type drop down menu.
4.
Choose Equation radio button
5.
Enter the following values in the corresponding fields:
X = 20 To X = 1000 Delta X = 20
Notice: We enter nothing in the Y field, therefore generating a 0 for the Y-Value at all X-Values, which creates a frequency range. Click OK, then...
6.
Click Cancel
What Create a function for the Response Spectrum Frequencies
How
Step
UI
Command/Display
19-8 1.
Generation of Response Spectra - Single Degree of Freedom model
Model, Function Menu
2.
In Function Definition dialog box:
3.
Type “Oscillator Damping” in Title field Select “0..Dimensionless” from Type drop down menu.
4.
Choose Single Value radio button (if not already selected)
5.
Enter the following values in the corresponding fields:
X = 0, Then…Click More button X = 0.05, Then…Click More button X = 0.10
Notice: We enter nothing in the Y field, therefore generating a 0 for the Y-Value at all X-Values, which creates different damping values Click OK, then…
6.
Click Cancel
Setting the Response Spectrum Generation Parameters The number of time steps, time per step, and selection of Response/Shock Spectrum Frequencies and Damping functions must be set in order for NX Nastran to run the analysis.
What Set the parameters for Response Spectra Generation
How
Step 1.
UI Menu
Command/Display Model, Load, Dynamic Analysis
Setting the Response Spectrum Generation Parameters
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Direct Transient radio button Enter the following values in the corresponding fields:
19-9
Number of Steps = 100 Time per Step = 0.0005 Output Interval = 1
4.
Notice: The Time per Step must be set to a value smaller than the time period of the sine pulse in order for the analysis to run. Select “2..Oscillator Frequencies” from the Frequencies drop down menu in the Response/Shock Spectrum section (left side of the dialog box)
Select “3..Oscillator Damping” from the Damping drop down menu in the Response/Shock Spectrum section (right side of the dialog box)
5.
Click OK
Creating a Group for Output Request needs
What Create a group containing a node in order to recover specific, requested output responses.
How
19-10
Step 1.
UI
Generation of Response Spectra - Single Degree of Freedom model
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Results Nodes” in the Title field Click OK
4.
Group, Node, ID Menu
5.
In Entity Selection – Select Node(s) for Group dialog box:
6.
Enter “1” into the ID field Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Setting up the Analysis Set Manager What Create an analysis case for Direct Transient Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
Type “Response Spectrum Gen” in the Title field
Setting up the Analysis Set Manager
4.
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “5..Response Spectrum” from the Analysis Type drop down menu
5.
Click Next button 7 times
6.
In NASTRAN Output for Response Spectrum Analysis dialog box:
7.
Choose Absolute radio button (if not already selected) CHECK T1 box next to Acceleration
8.
Click OK
9.
In Nodal Results dialog box:
Highlight “1..Results Nodes” from the Group selection list
19-11
19-12 10.
Generation of Response Spectra - Single Degree of Freedom model
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-processing - Response Spectrum Generation We have requested XY plotted data for the nodal accelerations for the node that we placed in our “Results Nodes” group. Our Oscillator Damping function will make sure that NX Nastran produces an acceleration plot at 0%, 5%, and 10% damping conditions. FEMAP will create functions representing this data. This data is available in the *.f06 print results file and NOT the *.op2 binary results file. Make sure to read in the *.f06 file in order to view the requested output.
What View the Acceleration results function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “5..ABSACC1 1 0.05” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK View, Options or…
6. Menu
Press the F6 Key or choose “options” from the view icon
on the View Toolbar
Post-processing - Response Spectrum Generation
19-13
7.
In View Options dialog box:
8.
Choose PostProcessing Radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
9.
Highlight “2..Log-Log” from the Plot Type selection list Click OK
The XY Plot of X-Acceleration at 5% damping should look like this:
This completes the Response Spectrum Generation example. Save the model as Spectrum.mod.
19-14
Generation of Response Spectra - Single Degree of Freedom model
Thermal Stress Analysis Mounting Plate 20.
Heat Transfer Analysis is used to determine the effects Conduction, Convection, and Radiation can have on a structure. Heat Transfer can occur during a Steady-Sate condition or over time with Transient Analysis. Material Properties, Heat Transfer Coefficients, and Heat Flux can be temperature dependent. Flow conditions can be set for Forced Convection, view factor calculations performed for Radiation analysis, as well as many other factors which help determine a system’s behavior when thermal conditions are involved. NX Nastran supports many options used in Heat Transfer analysis, many of which will be explored in this section of examples.
A mounting plate will be subject to a temperature of 250º F at same time another portion of the plate is being heated at 200º F. The ambient temperature of the plate and surroundings is 70º F. A temperature will be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. Those nodal temperatures will then become the loading condition for a static analysis to determine the thermal stress the mounting plate will encounter.
Mounting Plate
For this example we will be using a model of a mounting plate (with underlying geometry) that has already been created. The analysis process includes:
· creating an ambient temperature body load as well as nodal temperatures.
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· creating a load from the temperature results, as well as, defining pinned constraints
20-2
Thermal Stress Analysis - Mounting Plate
· analyzing the model with NX Nastran’s Static Solution Method and then post processing the stress results using FEMAP’s contour capabilities
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Heat_Transfer/HTPlate.neu Locate HTPlate.neu
Click Open
Neutral File Read Options dialog box:
Click OK
Creating the Thermal Boundary Conditions
20-3
Creating the Thermal Boundary Conditions The model needs to have an ambient temperature set with a body load. Then localized heating in the form of nodal temperatures will also be created.
What Creating the Temperature Body Load
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Thermal” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “70” into the Default Temperature (T) field
20-4
7.
Thermal Stress Analysis - Mounting Plate
Click OK
What Creating the Nodal Temperatures using the nodes’ associativity to the underlying geometric curves
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
In View Quick Options dialog box:
CHECK Curve box located in the Geometry section, then
3.
UNCHECK Element box located in the Mesh section Click Done
4.
This will make the curves visible and hide the elements, so the curves can be picked to create the nodal temperatures. (The curves don’t have to visible to pick them, but for this example it will aid in the selection) Model, Load, Nodal Menu
Creating the Thermal Boundary Conditions
5.
In Entity Selection – Enter Node(s) to Select dialog box
6.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
20-5
Choose the curve that makes up the lower right hand portion of the hole (curve 10)
Curve 9
Curve 10
7.
Click OK
8.
In Create Loads on Nodes dialog box
Highlight Temperature from the selection list 9.
Enter “200” into the Temperature field
10.
Click OK
In Entity Selection – Enter Node(s) to Select dialog box
11.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
Choose the curve that makes up the upper left hand portion of the hole (curve 9) 12.
Click OK
13.
Enter “250” into the Temperature field
20-6 14.
Thermal Stress Analysis - Mounting Plate
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
15.
Choose the 12 curves that make up the outside perimeter of the plate (curves clockwise from top right: 3, 36, 32, 2, 37, 17, 1, 38, 26, 4, 35, 16)
16
35
3
36
4
32
26
2
38
1
16.
Click OK
17.
Enter “70” into the Temperature field
18.
Click OK, then…
17
Click Cancel What View the model with the elements and applied nodal temperatures visible
How
Step 1.
UI Crtl-Q
Command/Display This will bring up the View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
37
Running the Steady-State Thermal Analysis
20-7
2.
CHECK Element box located in the Mesh section, and Thermal box in the Loads section, then…
3.
UNCHECK Curves box located in the Geometry section Click Done
THE THERMAL MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Thermal Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
20-8 5.
Thermal Stress Analysis - Mounting Plate
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the Plate is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “1..Case 1 Time 1.” from Output Set drop down menu
5.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK
Creating Nodal Temperatures from the Thermal Results
20-9
The contour plot of the temperatures should look like this:
Creating Nodal Temperatures from the Thermal Results The results of the Thermal analysis will used to thermally “load” the plate for a static analysis which will produce a stress value after the model has been constrained.
What Create the Nodal Temperature on all nodes
How
Step 1.
UI
Command/Display Model, Load, From Output
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
Choose Temperature radio button in the Nodal Loads section
20-10
Thermal Stress Analysis - Mounting Plate
3.
Click OK
4.
In Create Loads From Output dialog box:
Select “1..Case 1 Time 1” from Output Set drop down menu
Select “31..Temperature” from X Vector drop down menu Click OK, then…
5.
In the “OK to Update Existing Temperatures” message window:
Click Yes button Creating the Constraints
What Create pinned nodal constraints
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating Nodal Temperatures from the Thermal Results
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Pinned” in the Title field Click OK
4.
20-11
Model, Constraint, Nodal Menu
5.
In Entity Selection – Enter Node(s) to Select dialog box
6.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
Choose the 12 curves that make up the outside perimeter of the plate (curves clockwise from top right: 3, 36, 32, 2, 37, 17, 1, 38, 26, 4, 35, 16)
Notice: Because the same exact curves are being picked for this step as where chosen the last time the Entity Selection dialog box was used, the Previous button can be clicked and the curves will be selected again.
16
35
3
36
4
32
26
2
38
1
17
37
20-12 7.
Thermal Stress Analysis - Mounting Plate
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Pinned button, then…
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel What View the model with the elements and constraints visible
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
CHECK Constraint box located in the Others section, then…
3.
UNCHECK Thermal box in the Loads section Click Done
THE THERMAL STRESS MODEL IS NOW READY TO BE ANALYZED!
Running the Thermal Stress Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
Post-Processing the Thermal Results
1.
20-13
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Thermal Stress” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “1..Static” from the Analysis Type drop down menu
5.
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Static Analysis has created stress results. The best way to view the stress of the Plate is with a contour plot.
What View the stress results in a FEMAP contour plot
How
Step
UI
Command/Display
20-14 1.
Thermal Stress Analysis - Mounting Plate
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Contour radio button in Contour Style section (if not already chosen) Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box: Select “2.. NASTRAN Case 1” from Output Set drop down menu
You will see this box:
5.
, Click OK
Select “7033..Plate Top VonMises Stress” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK The contour plot of the stress should look like this:
This Concludes the Thermal Stress Analysis example. It is recommended to save the model file.
Steady - State Thermal Analysis Circuit Board 21.
A circuit board will be subject to a heat generation loads being created by different sized chips on the board. The temperature of the back side of the plate is 45º C and the ambient temperature of the system is 25º C. The “board” is made of a composite material, and the chips are made of a material with a higher conductivity. A temperature will be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. This model will be used to demonstrate other Heat Transfer capabilities for the next few examples.
Circuit Board
For this example we will be using a model of a circuit board that has already been created including the materials and properties. The analysis process includes:
· creating an ambient temperature body load, as well as, heat generation loads and nodal temperatures.
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements using the section cut and multiple dynamic cutting plane post-processing features of FEMAP.
Importing the Model What
21-2
Steady - State Thermal Analysis - Circuit Board
Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Heat_Transfer/HTBoard.neu Locate HTBoard.neu
Click Open
Neutral File Read Options dialog box:
Click OK
Examining the Material Properties for Thermal Analysis
What Look at the existing material properties in the model
Importing the Model
21-3
How
Step 1.
UI
Command/Display Modify, Edit, Material
Menu
2.
In Entity Selection – Select Material(s) to Edit dialog box: Click Select All button, then…
Click OK
Notice: This step is here to take a look at the values that should be entered at a minimum for any thermal analysis. Please, DO NOT CHANGE THE VALUES or the results of the analysis will be altered and not match those in the example. Also, instead of using the Modify, Edit, Material command, the List, Model, Material command can be used to view the values in the message box located below the main graphics window.
The values of the material are in the following units:
Conductivity, K = W/cmº C Specific Heat, Cp = kJ/kgº C Density (rho) = kg/cm3
21-4 3.
Steady - State Thermal Analysis - Circuit Board
In the Define Material - ISOTROPIC dialog box:
Click OK, then…
View the values for the “Chips” material, then…
Click OK
Creating the Heat Generation Loads and Thermal Boundary Conditions Each “chip” will generate a different amount of heat. The heat generation loads will be placed at the center node of each chip to create an even distribution through the chip The model needs to have an ambient temperature set with a body load and nodal temperatures on the backside of the board. What Creating the Temperature Body Load How Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Heat Generation” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “25” into the Default Temperature (T) field
Creating the Heat Generation Loads and Thermal Boundary Conditions
7.
Click OK
What Creating the Heat Generation loads at the center of each “chip” How Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 378 at center of the large chip
Node 378
Node 434
Node 408
21-5
21-6
Steady - State Thermal Analysis - Circuit Board
3.
Click OK
4.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 5.
Enter “0.12” into the Generation field (The units are in watts)
6.
Click OK
7.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 434 at center of the taller small chip 8.
Click OK
9.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 10.
Enter “0.10” into the Generation field (The units are in watts)
11.
Click OK
12.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 408 at center of the shorter small chip 13.
Click OK
14.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 15.
Enter “0.08” into the Generation field (The units are in watts)
16.
Click OK, then…
Click Cancel What
Creating the nodal temperatures on the backside of the circuit board
Creating the Heat Generation Loads and Thermal Boundary Conditions
21-7
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click ZX Front button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
3.
Model, Load, Nodal Menu
4.
Entity Selection – Enter Node(s) to Select dialog box
Select Nodes on the backside of the circuit board by holding down the shift key, clicking and dragging the mouse to create a box select around the nodes
Box Selection 5.
Click OK
21-8 6.
Steady - State Thermal Analysis - Circuit Board
In Create Loads on Nodes dialog box
Highlight Temperature from the selection list 7.
Enter “45” into the Temperature field (Units are in º C)
8.
Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Circuit Board” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
Post-Processing the Thermal Results
5.
21-9
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the circuit board is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK View, Select or…
3. Menu
4.
Press the F5 Key or choose the view select icon In View Select dialog box:
5.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
6.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “1..Case 1 Time 1.” from Output Set drop down menu
Select “31..Temperature” from Contour drop down menu located in Output Vectors section
21-10 7.
Steady - State Thermal Analysis - Circuit Board
Click OK
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Viewing the internal temperature results can be useful. This can be accomplished by using an Advanced FEMAP Post-Processing feature called Dynamic Cutting Plane which creates a cross-section view of solid element results.
What Utilize FEMAP’s Dynamic Cutting Plane Feature
How
Step 1.
UI Menu
Command/Display View, Advanced Post, Dynamic Cutting Plane
Post-Processing the Thermal Results
2.
21-11
In Dynamic Section Cut Control dialog box:
There is a “slider bar” that can be moved right or left to move the selected cutting plane through the model. The cutting plane can be specified using the Plane button in the dialog box.
Click Plane button
3.
In Plane Locate – Define Primary Cutting Plane dialog box:
4.
Click Method button and highlight Global Plane In Global Plane – Define Primary Cutting Plane dialog box:
5.
Choose YZ Plane radio button Click OK, then…
Move the slider bar back and forth and the model will be cut away as it moves. Stop the bar when the number in the Value field is near 2.5 The Plot should appear something like this:
6.
In Dynamic Section Cut Control dialog box:
Click OK
What
21-12
Steady - State Thermal Analysis - Circuit Board
Create Multiple Cutting Planes for use with FEMAP’s Dynamic Cutting Plane Feature
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Section Cut radio button in Contour Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
5.
Choose Multiple Sections radio button in Section Cut Options section CHECK Section boxes 2 and 3 located in the Section Cut Options section
6.
Click Section 2 Button
7.
In Global Plane – Define Primary Cutting Plane dialog box:
8.
Choose ZX Plane radio button Click OK, then
In Selecting PostProcessing Data dialog box:
9.
Click Section 3 Button In Global Plane – Define Primary Cutting Plane dialog box:
10.
Choose XY Plane radio button Click OK, then…
In Selecting PostProcessing Data dialog box:
Click OK, then…
In View Select dialog box:
Click OK
Post-Processing the Thermal Results
11.
21-13
View, Advanced Post, Dynamic Cutting Plane Menu
12.
In Dynamic Section Cut Control dialog box:
The 1,2,and 3 Section radio buttons are now available for picking
Click the different radio buttons to be able to move the corresponding section planes through the model
Try this: Take Section 1 to a value near 1.5, Section 2 near 2.6, and Section 3 near.175 The Plot should resemble this:
13.
In Dynamic Section Cut Control dialog box:
Click OK
This Concludes the Circuit Board Heat Generation Analysis example. Please save the model file as HTBoard.mod for use in later examples such as Free Convection.
21-14
Steady - State Thermal Analysis - Circuit Board
Steady - State Thermal Analysis Free Convection 22.
The same circuit board will be subject to the same loading conditions as in the last example, but this time Free Convection will be used to allow heat to transfer between the top of the board and the surroundings. By taking Free Convection into account, the temperature will again be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. The temperatures on the circuit board based on the Conduction only conditions that existed in the last example are worst case because heat was not able to transfer to the surroundings using Free Convection.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating a Free Convection thermal condition on the top surface of the circuit board
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements and the contour plot of the Convection Surface using groups
Opening an Existing FEMAP Model What Open an existing FEMAP model file HTBoard.mod.
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Heat_Transfer/HTBoard.mod
Click Open
22-2
Steady - State Thermal Analysis - Free Convection
If the circuit board model is showing any contours or section cuts, Press the F5 button on the keyboard, then choose the None – Model Only radio button in the Contour Style section and Click OK.
The model should only be showing elements and thermal loads to begin the example.
Creating the Free Convection Boundary Conditions The top surface of the circuit board will allow Free Convection to the surroundings. It is required to have a convection heat transfer coefficient (h) in order to create the proper effects due to free convection. For this example we will use h = 4.1 x 105 W/mm2 º C.
What Create the Free Convection Boundary Condition
How
Step 1.
UI
Command/Display Model, Load, Elemental
Menu
2.
Entity Selection – Enter Elements(s) to Select dialog box
Click Select All button, then…
Click OK
Creating the Free Convection Boundary Conditions
3.
22-3
In Create Loads on Elements dialog box
Highlight Convection from the selection list 4.
Enter “4.1E-5” into the Coefficient field, then…
5.
Enter “25” in the Temperature field Click OK
6.
In Face Selection for Elemental Loads dialog box:
7.
Choose Adjacent Faces radio button in Method section, then… Click in Face field to activate
Select the top Element face of ANY Element on the top surface of the circuit board (not the chips)…for example face 2 on Element 82
Element 82
22-4 8.
Steady - State Thermal Analysis - Free Convection
Click OK, then…
Click Cancel
Notice: Creating this type of convection condition will actually create plot-only planer elements on the model and FEMAP will require the model be saved during the Analyze step for proper post-processing.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Use an existing analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
Post-Processing the Thermal Results
2.
22-5
In Analysis Set Manager dialog box:
Click Analyze button
Notice: An analysis should already exist in HTBoard.mod. If one does not, please follow the Running the Steady-State Thermal Analysis section from Example 21.
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the circuit board is with a contour plot. The Elemental Free Convection values can also be viewed with a contour plot of a selected group.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
3.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
22-6
Steady - State Thermal Analysis - Free Convection
4.
In View Quick Options dialog box:
5.
Click All Entities Off button CHECK Element box located in the Mesh section
6.
Click Done
7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
9.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Notice the Maximum Nodal Temperature is lower due to the effects of free convection
Post-Processing the Thermal Results
22-7
What View the temperature results in a FEMAP animation
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Animate radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
Select “31..Temperature” from Deformation and Contour drop down menus located in Output Vectors section
5.
Notice: FEMAP needs a deformation vector to animate a contour plot, therefore use Temperature as the deformation vector. The Temperature will not actually be used deform the model, but a deformation vector does need to be selected. Click OK
6.
In View Select dialog box:
7.
CHECK Skip Deformation box Click OK
The speed of the animation can be controlled by using the View, Advanced Post, Animation command while the Model is animating. Click the Slower and Faster buttons until the desired viewing speed has been found
Creating a Group for viewing purposes
What Create a group containing an element type in order to view contours on the Convection Surface only.
How
22-8
Step 1.
UI
Steady - State Thermal Analysis - Free Convection
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Convection Surface” in the Title field Click OK
4.
Group, Element, Type Menu
5.
In Entity Selection – Select Element Types for Group dialog box:
Select “32..L Plot Planar” from Type drop down menu
Notice: Remember that FEMAP created these Plot-planer elements to be used with the Convection “loading” condition Click OK
6. 7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
on the View Toolbar
9.
Choose None - Model Only radio button in Deformed Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “80031..Elem Free Convection” from Contour drop down menu located in Output Vectors section Click OK, then…
In View Select dialog box:
Click Model Data button
Post-Processing the Thermal Results
12.
In Select Model Data for View dialog box:
13.
Choose Active radio button Group section Click OK, then…
22-9
In View Select dialog box:
Click OK The Plot of the Free Convection values should look like this:
This Concludes the Circuit Board Free Convection example. Please save the model file as HTFree.mod.
22-10
Steady - State Thermal Analysis - Free Convection
Temperature - Dependent effects Circuit Board 23.
The same circuit board will be subject to the same loading conditions as in the last two examples, but this time the conductivity of the Material Property of the chips will be temperature dependent, as well as, the Convection Coefficient.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating functions to represent temperature-dependence for the Conductivity of the Chips and for the Free Convection Coefficient
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements and the contour plot.
Opening an Existing FEMAP Model What Open an existing FEMAP model file HTBoard.mod.
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Heat_Transfer/Temperature Dependent Circuit/HTBoard.mod
Click Open
23-2
Temperature - Dependent effects - Circuit Board
Use the View, Select command. Choose None-Model Only for both Contour Style and Deformed Style. Then Click OK.
Creating a Temperature Dependent Material Property A function will be created to define the relationship between Temperature and Conductivity for the “Chips” Material Property. This function will then be referenced by the Material Property using a portion of the Define Material dialog box.
What Create Conductivity vs. Temperature (k vs. T) function How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Chips (k vs. T)” in the Title field Select “2..vs. Temperature” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 10, Y = 0.333, Then…Click More button X = 30, Y = 0.386, Then…Click More button X = 50, Y = 0.415, Then…Click More button X = 70, Y = 0.437, Then…Click More button X = 90, Y = 0.452, Then…Click More button X = 120, Y = 0.461, Then…Click More button X = 200, Y = 0.461
Creating a Temperature Dependent Material Property
6.
23-3
Click OK, then
Click Cancel
What View Conductivity vs. Temperature (k vs. T) function using FEMAP’s XY Plot Capabilities How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
on the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..Chips (k vs. T)” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key)
23-4
Temperature - Dependent effects - Circuit Board
The XY Plot should look like this:
What Modify the Chips Material Property to reference the k vs. T function
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Quick Hidden Line radio button Click OK button
4.
Modify, Edit, Material Menu
5.
Entity Selection – Select Material(s) to Edit dialog box:
Select any element on one of the “Chips”
on the View Toolbar
Creating a Temperature Dependent Convection Coefficient (h)
6.
23-5
Click OK, then…
Tip: You can also edit an existing Material using the Edit command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight any existing Material, then right mouse click to see the context sensitive menu). In this case, you would highlight “1..Chips” in the list in the Materials branch, then right click and choose Edit. In the Define Material - ISOTROPIC dialog box:
7.
Click the Function References tab
Notice: The Message at the top of the Function References portion of the dialog box, “Press CtrlF in each field to select from a list of the available functions”, explains an easy way to choose the desired function for all fields that will have function-dependence. Be sure to have the proper field reference the correct function.
8.
Ctrl-F
Click in the Conductivity, K field, making it active In Select Function dialog box:
9.
Highlight 1..Chips (k vs. T) from the selection list Click OK
10.
In the Define Material - ISOTROPIC dialog box:
Click the General tab
11.
Click in the Conductivity, K field, making it active Enter “1.0” in the Conductivity, k field (1.0 * function value)
12.
Click OK
Creating a Temperature Dependent Convection Coefficient (h) A function will be created to define the relationship between Temperature and Free Convection Coefficient. This function will then be referenced by the Convection “loads”.
What Create Convection Coefficient vs. Temperature (h vs. T) function
23-6
Temperature - Dependent effects - Circuit Board
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Convection Coeff” in the Title field Select “2..vs. Temperature” from Type drop down menu.
4.
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 10, Y = 1.2E-5, Then…Click More button X = 30, Y =5.3E-5, Then…Click More button X = 50, Y = 8.9E-5, Then…Click More button X = 70, Y = 1.2E-4, Then…Click More button X = 90, Y = 3.1E-4, Then…Click More button X = 120, Y = 5.1E-4, Then…Click More button X = 200, Y = 5.1E-4 Click OK, then…
6.
Click Cancel
What Create the Free Convection Boundary Condition
How
Step 1.
UI Menu
Command/Display Model, Load, Elemental
Creating a Temperature Dependent Convection Coefficient (h)
2.
23-7
Entity Selection – Enter Element(s) to Select dialog box
Click Select All button, then…
3.
Click OK In Create Loads on Elements dialog box
Highlight Convection from the selection list 4.
Enter “1.0” into the Coefficient field, then…
5.
Enter “25” in the Temperature field Select “2..Convection Coeff” from Time/Freq Dependence drop down menu located next to the Coefficient field
6.
Click OK
7.
In Face Selection for Elemental Loads dialog box:
8.
Choose Adjacent Faces radio button in Method section, then… Click in Face field to activate
Select the top Element face of ANY Element on the top surface of the circuit board (not the chips)…for example face 2 on Element 82
Element 82
23-8
9.
Temperature - Dependent effects - Circuit Board
Click OK, then…
Click Cancel
Notice: Creating this type of convection condition will actually create plot-only planer elements on the model and FEMAP will require the model be saved during the Analyze step for proper post-processing.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
Post-Processing the Thermal Results
23-9
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
Click Analyze button
Notice: An analysis should already exist in HTBoard.mod. If one does not, please follow the Running the Steady-State Thermal Analysis section from Example 21.
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution based on the Temperature Dependency across the circuit board is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
23-10 3.
Crtl-Q
Temperature - Dependent effects - Circuit Board
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 4.
In View Quick Options dialog box:
5.
Click All Entities Off button CHECK Element box located in the Mesh section
6.
Click Done
7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
9.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK, then...
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Post-Processing the Thermal Results
23-11
The Maximum temperature is lower than the two previous examples due to the representing the Material properties and Convection Coefficient with a higher degree of accuracy and realism.
Using the Dynamic Isosurface Feature of FEMAP
The Dynamic Isosurface is utilized to show areas of identical results values throughout a model containing solid elements. In this case, the results values of interest are temperatures and this feature will always use the selected Contour Output Vector to create the isosurfaces.
What
Utilize the Dynamic IsoSurface feature of FEMAP How
Step 1.
UI
Command/Display View, Advanced Post, Dynamic IsoSurface
Menu
2.
In Dynamic IsoSurface Control dialog box:
There is a “slider bar” that can be moved right or left to move the isosurface through the model to view the areas of identical value
3.
Move the bar through the entire rang of values (from left to right). After seeing the entire range of values, try moving the slider bar until the value reaches just above 45, 60, 75, and 95 to examine the different isosurface at each value. Then… Click OK
The model should be contoured fully again.
This Concludes the Circuit Board with Temperature Dependent Factors Analysis example. Please save the model file as HTTDBoard.mod.
23-12
Temperature - Dependent effects - Circuit Board
24.
Enclosure Radiation
Three plates will be used for this simple example of Enclosure Radiation. The plates on each side “Can be shaded” and the center plate “Can shade” the other two. An Emissivity Value will be assigned to each “face” of the plates that will be involved in the analysis. The geometry will be created using FEMAP.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating geometry to represent the plates, then meshing the model with parabolic elements
· assigning Emissivity values and applying heat flux to the model
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing contour plots of the nodal temperature results
Opening a FEMAP Model What Open a new FEMAP model file.
How
Step 1.
UI
Command/Display File, New
Menu
Creating the Geometry
Three surfaces must be created for this model.
What Create the surfaces
24-2
Enclosure Radiation
How
Step 1.
UI
Command/Display Geometry, Surface, Corners
Menu
2.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = 0, Then…Click OK button X = 5, Y = 0, Z = 0, Then…Click OK button X = 5, Y = 5, Z = 0, Then…Click OK button X = 0, Y = 5, Z = 0, Then…Click OK button 3.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = 4, Then…Click OK button X = 5, Y = 0, Z = 4, Then…Click OK button X = 5, Y = 5, Z = 4, Then…Click OK button X = 0, Y = 5, Z = 4, Then…Click OK button 4.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = -3, Then…Click OK button X = 5, Y = 0, Z = -3, Then…Click OK button X = 5, Y = 5, Z = -3, Then…Click OK button X = 0, Y = 5, Z = -3, 5.
Click OK, then
Click Cancel
Creating Materials and Properties
Creating Materials and Properties
What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
In Define Material - ISOTROPIC dialog box:
Type “Plates” in Title field, then…
Enter “237” in Conductivity, k field (units: W/m º K)
Enter “903” in Specific Heat, Cp field (units: J/kg º K)
Enter “2702” in Mass Density field (units: kg/m3) Click OK, then…
3.
Click Cancel
What Create a Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – PLATE Element Type dialog box:
Type “Plates” in Title field, then…
3.
Enter “0.001” in Thicknesses, Tavg or T1 field Select “Plates” from the Material drop down menu
24-3
24-4
Enclosure Radiation
4.
Click Elem/Property button
5.
In Element / Property Type dialog box:
CHECK Parabolic Elements at the top of the dialog box
Notice: This will create second order elements (parabolic) with mid-side nodes when the plates are meshed. Click OK, then…
6.
In Define Property – PLATE Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Plates
What Set the mesh size
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Default Size
Menu
2.
In Default Mesh Size dialog box:
3.
Enter “1” in both the Size and Min Elem fields, Click OK
What Mesh the plates
How
Step
UI
Command/Display
Creating Materials and Properties
1.
24-5
Mesh, Geometry, Surface Menu
2.
In Entity Selection – Select Surfaces to Mesh dialog box:
Click Select All button, then…
3.
Click OK In Automesh Surfaces dialog box:
4.
Select “Plates” from the Property drop down menu CHECK Midside Nodes on Geometry box
5.
Click OK
6.
View, Rotate, Model or… Menu
Press the F8 Key 7.
In View Rotate dialog box:
Click Isometric button, then…
Click OK Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
8.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 9.
In View Quick Options dialog box:
Click All Entities Off button, then
10.
Click Loads/Constraints On button CHECK Element box located in the Mesh section
24-6 11.
Enclosure Radiation
Click Done
The model should now look like this:
Reversing the Element Normals The plate elements have two “faces” each. Because the model is representing an enclosure, the normals of the elements on the two outer surfaces must point towards the middle surface. First the element normals need to be turned on in order to see which elements are not pointing towards the center. Next the elements with normals not facing the middle plate will be modified.
What View the Element Normals
How
Step 1.
UI
Command/Display View, Options or…
Menu
2.
3.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose Labels, Entities and Color radio button under Category Highlight “Element - Directions” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “1..Normal Vectors” from the Normal Style selection list
Reversing the Element Normals
4.
CHECK Show Direction box in upper right corner of dialog box
5.
Click OK
The normal vector should now be visible:
Element Normals need to be reversed on left plate
The normal vectors need to be reversed on the left plate while in Isometric View (shown) What Reverse the element normals
How
24-7
24-8
Step 1.
UI
Enclosure Radiation
Command/Display Modify, Update Elements, Reverse Normal/Orient First Edge
Menu
2.
In Entity Selection – Select Element(s) to Update Direction dialog box:
3.
Click Method button and highlight On Surface Entity Selection – Select Element(s) to Update Direction (On Surfaces)
Choose the surface on the left side of the graphics window (Surface 2) 4.
Click OK
5.
In Update Element Directions dialog box:
Choose Reverse Element Direction radio button
6. 7.
Click OK Ctrl-G
Window, Regenerate (This will Regenerate the model in order to see the changes)
The Model should now look like this:
Creating Radiation Emissivity and Heat Flux Loads
24-9
Creating Radiation Emissivity and Heat Flux Loads Because the middle surface will need to radiate to both other surfaces an Emissivity value needs to be placed on both “faces” of the middle surfaces elements. The Emissivity values are created by “loading the face” of the elements and defining whether the elements “Can Shade” or “Can be Shaded” after the selection of the Enclosure Radiation option.
What Create a load set and Body Load
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Radiation” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “475” into the Default Temperature (T) field
7.
Click OK
What Create Radiation settings
How
Step 1.
UI Menu
Command/Display Model, Load, Heat Transfer
24-10 2.
Enclosure Radiation
In Heat Transfer Loads dialog box:
Enter “5.670E-8” in the Stefan-Boltzmann field (units: W/m2º K4)
3.
Click OK
What Create Radiation “loads”
How
Step 1.
UI
Command/Display Model, Load, Elemental
Menu
2.
In Entity Selection – Enter Elements(s) to Select dialog box
3.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the left hand surface (Surface 2) 4.
Click OK
Creating Radiation Emissivity and Heat Flux Loads
5.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 6.
CHECK Enclosure Radiation box, then… Can Be Shaded box
7.
Enter “1.0” into the Emissivity field
8.
Click OK
9.
In Face Selection for Elemental Loads dialog box
Enter “1” into the Face field
24-11
24-12 10.
Enclosure Radiation
Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
11.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the right hand surface (Surface 3) 12.
Click OK
13.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 14.
CHECK Enclosure Radiation box, then… Can Be Shaded box
15.
Enter “1.0” into the Emissivity field
16.
Click OK
17.
In Face Selection for Elemental Loads dialog box
18.
Enter “1” into the Face field Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
19.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the middle surface (Surface 1) 20.
Click OK
21.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 22.
CHECK Enclosure Radiation box, then… Can Shade box
23.
Enter “1.0” into the Emissivity field
24.
Click OK
Creating Radiation Emissivity and Heat Flux Loads
25.
In Face Selection for Elemental Loads dialog box
26.
Enter “1” into the Face field Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
27.
Choose the surface on the middle surface (Surface 1) 28.
Click OK
29.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 30.
CHECK Enclosure Radiation box, then… Can Shade box
31.
Enter “1.0” into the Emissivity field
32.
Click OK
33.
In Face Selection for Elemental Loads dialog box
34.
Enter “2” into the Face field Click OK, then…
Click Cancel What Create Heat Flux Load on element
How
Step 1.
UI Menu
Command/Display Model, Load, Elemental
24-13
24-14 2.
Enclosure Radiation
Entity Selection – Enter Element(s) to Select
Choose the center element on the middle surface (Element 13)
Element 13
3.
Click OK
4.
In Create Loads on Elements dialog box
Highlight Heat Flux from the selection list 5.
Enter “1200” into the Flux field
6.
Click OK
7.
In Face Selection for Elemental Loads dialog box
8.
Enter “1” into the Face field Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Post-Processing the Thermal Results
Step 1.
UI
24-15
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Radiation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
5.
Click Next 7 times
6
In Boundary Conditions dialog box:
7.
Select “1..Radiation” from Load AND Initial Conditions drop down menus Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Radiation Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the Plate is with a contour plot.
What
24-16
Enclosure Radiation
Create a group
How
Step 1.
UI
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Parabolic Elements” in the Title field Click OK
4.
Group, Element, Type Menu
5.
In Entity Selection – Select Element Types for Group dialog box:
Select “18..P Plate” from Type drop down menu
Notice: This will allow better viewing of the plate element results Click OK
6.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
on the View Toolbar
Post-Processing the Thermal Results
4.
24-17
In Selecting PostProcessing Data dialog box:
Select “1..Case 1 Time 1.” from Output Set drop down menu
5.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK, then…
In View Select dialog box:
6.
Click Model Data button In Select Model Data for View dialog box:
7.
Choose Active radio button Group section Click OK, then…
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Notice that the plate further away from the middle plate has a lower temperature.
This Concludes the Enclosure Radiation example. Please save the model file as Radiation.mod.
24-18
Enclosure Radiation
Plastic Deformation of Rod Nonlinear Material 25.
A simple rod model will be built out of a material which will become nonlinear after the model reaches a defined yield criteria (von Mises Stress). The model will be loaded axially beyond the yield stress and then unloaded. These loading conditions will leave the rod plastically deformed. The displacement and strain results will then be viewed with an XY plot.
For this example a model made of rod elements will be created using FEMAP. The analysis process includes:
· creating a function to represent a strain vs. stress curve and use it to define a nonlinear material
· creating the mesh, loads, and boundary conditions
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the displacements and strains using FEMAP’s XY Plotting Capabilities
Open a New FEMAP Model File
Creating the Nonlinear Material What Create a simple stress vs. strain function
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Strain vs. Stress” in the Title field Select “4..vs. Stress” from Type drop down menu.
25-2
Plastic Deformation of Rod - Nonlinear Material
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0, Then…Click More button X = 180, Y = 0.001, Then…Click More button X = 235, Y = 0.003, Then…Click More button X = 270, Y = 0.005 Click OK, then...
6.
Click Cancel Visual verification of the Strain vs. Stress curve (or any function) is always a good idea.
What Verify the Stress vs. Strain curve using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..Strain vs. Stress” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK
from the View Toolbar
Creating the Nonlinear Material
25-3
Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key) View, Options or…
6. Menu
7.
8.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “XY Curve 1” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Output Values” from Data Labels selection list
Highlight “Lines with Points” from Curve Style selection list
25-4 9.
Plastic Deformation of Rod - Nonlinear Material
Click OK
The Stress vs. Strain Curve should look like this:
What Create the Material
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Draw Model radio button Click OK
4.
Model, Material Menu
from the View Toolbar
Creating the Property and Mesh
5.
25-5
In Define Material - ISOTROPIC dialog box:
Type “Nonlinear Material” in Title field, then…
Enter “200,000” in Young’s Modulus, E field (units: N/mm2)
6.
Enter “0.3” in Poisson’s Ratio, nu field Click Nonlinear tab
7.
In the Nonlinear portion of the Define Material - ISOTROPIC dialog box:
8.
Choose Plastic radio button Select “1..Strain vs. Stress” from Time/Freq Dependence drop down menu located in the Nonlinear Properties section
9.
Select “0..von Mises” from the Yield Criterion drop down menu in the Yield Function section Enter “180” in Initial Yield Stress field
10.
Click General tab of the Define Material - ISOTROPIC dialog box
11.
Click OK, then…
Click Cancel
Creating the Property and Mesh What Create a Property
How
Step 1.
UI Menu
Command/Display Model, Property
25-6
Plastic Deformation of Rod - Nonlinear Material
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Rod radio button in Line Elements section Click OK
5.
In Define Property – ROD Element Type dialog box:
Type “Rod” in Title field
6.
Enter “1” in Area, A field Select “Nonlinear Material” from Material drop down menu
7.
Click OK, then…
Click Cancel What Create the Nodes and Elements
How
Step 1.
UI
Command/Display Mesh, Between
Menu
2.
In Generate Between Corners dialog box:
3.
Select “Rod” from the Property drop down menu Enter “11” in #Nodes field
4.
Click OK
Creating Loads and Constraints
5.
25-7
In the Locate – Enter Corner 1 of Mesh (Cancel to Abort or Backup) dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 100, Y = 0, Z = 0 Click OK
6.
Creating Loads and Constraints Two Load Sets must be created in order to simulate a loading condition and an “unloaded” condition. A load does need to be applied for the unloaded condition for the analysis to run, so a very small load will be applied axially in a second load set to accomplish the “relaxation” of the rod.
What Create the fixed constraint
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the node at the left side end of the rod (Nodes 1)
25-8 6.
Plastic Deformation of Rod - Nonlinear Material
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
7.
Click OK, then… In Entity Selection – Enter Node(s) to Select dialog box:
8.
Click Cancel View, Autoscale, Visible Menu
OR Press Ctrl - A What Creating the “Loading” Load Set
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Loaded” in the Title field Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the rod (Nodes 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list
Creating Loads and Constraints
8.
Enter “300” in FX field (units: N)
9.
Click OK, then…
Click Cancel What Creating the “Unloading” Load Set
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
Enter “2” in ID field
Type “Unloaded” in the Title field Click OK
3. 4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the rod (Nodes 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “0.001” in FX field (units: N)
9.
Click OK, then…
Click Cancel
What Create Nonlinear Static settings (They must be set for BOTH Load Sets)
25-9
25-10
Plastic Deformation of Rod - Nonlinear Material
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
Running the Nonlinear Static Analysis with two cases
7.
25-11
Model, Load, Set Menu
8.
In Create or Activate Load Set dialog box:
Highlight “1..Loaded” from the list 9.
Click OK
10.
Model, Load, Nonlinear Analysis Menu
11.
In Load Set Options for Nonlinear Analysis dialog box:
12.
Choose Static radio button Click Copy button
13.
Notice: This will copy the values of this dialog box that have been entered in another selected Load Set into the Active Load Set In Create or Activate Load Set dialog box:
Highlight “2..Unloaded” from the list 14.
Click OK, then…
In Load Set Options for Nonlinear Analysis dialog box:
Click OK THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis with two cases What Create an analysis set with multiple cases for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
25-12 1.
Plastic Deformation of Rod - Nonlinear Material
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Plastic Deformation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next 7 times
6.
In Nastran Output Requests dialog box:
7.
CHECK Strain in the Elemental Section Click OK, then…
In Analysis Set Manager dialog box:
Click Multi-Set button
Running the Nonlinear Static Analysis with two cases
8.
25-13
In Entity Selection – Select Constraint Set(s) to Generate Cases dialog box:
Click Select All, then…
Click OK
9.
In Entity Selection – Select Load Set(s) to Generate Cases dialog box:
Click Select All, then…
Click OK
10.
In Analysis Set Manager dialog box:
Double Click the words “Analysis Set: 1..Plastic Deformation” or click the “+” sign to the left of them.
The Analysis Set Manager Tree Structure will expand to show the different sections of the load case (Solution Options, Options, Master Control and Requests, Cases)
Two cases have been created: (Case names based on Load and constraint sets) Case: 1..Fixed – Loaded Case: 2..Fixed – Unloaded
Notice: All dialog boxes in the Analysis Set Manager can also be reached through the Tree Structure.
25-14
Plastic Deformation of Rod - Nonlinear Material
New Analysis Cases
11.
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”... Click Yes
Post-Processing the Results A multi-set animation of the results would show the plastic deformation, but due to the relatively small displacements in this model, a XY plot of the displacements and strain values would create a clearer method to visualize this results.
What Create a XY Plot of displacement of a single node of the rod over all the output sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Post-Processing the Results
2.
In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
25-15
Select “1..Case 1 Time 0.1” from drop down menu located in the Output Set section, then…
5.
Select “1..Total Translation” from drop down menu located in the Output Vector section Enter “11” in the Node field located in the Output Location section
6.
Leave the From and To fields in Show Output Set Section bank to plot the Output Vector over the range of the analysis Click OK, then…
In View Select dialog box:
Click OK The Plot of Node 11’s Total Translation should look like this:
What Create a XY Plot of plastic strain of a single element of the rod over all the output sets
25-16
Plastic Deformation of Rod - Nonlinear Material
How
Step 1.
2.
UI
Command/Display Right click in the Graphics window and choose XY Data from the menu
In Select XY Curve Data dialog box:
Select “1..Case 1 Time 0.1” from drop down menu located in the Output Set section, then…
3.
Select “3286..Rod Plastic Strain” from drop down menu located in the Output Vector section Enter “10” in the Element field located in the Output Location section
4.
Click OK
The Plot of Element 10’s Plastic Strain should look like this:
This Concludes the Large Deformation example. It is recommended to save the model file.
26.
Gap Contact - Cantilever Beam
A cantilever beams with a tubular cross section will be used to demonstrate Gap Contact found in Nonlinear Static Analysis. The beam will have one end fixed, and the free end will be loaded with a Force. During the analysis, the deformation of the model will cause the gap to close creating contact. Contact in analysis almost always signals the use of a nonlinear solution. This example will use the Nonlinear Static solving capability of NX Nastran.
For this example a beam model will be created using FEMAP. The analysis process includes:
· creating a beam property, meshing an existing curve
· creating a Gap property and the gap element, then loads and constraints
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the stresses on the beam using FEMAP’s Beam Diagram post-processing capability
Creating the Geometry What Create lines to represent the beams
How
Step 1.
UI
Command/Display File, New
Menu
2.
Geometry, Curve-Line, Coordinates Menu
26-2 3.
Gap Contact - Cantilever Beam
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 10, Y = 0, Z = 0 Click OK, then…
4.
Click Cancel, then press Ctrl-A to Autoscale the visible parts of the model
Creating the Materials and Properties What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). In Define Material - ISOTROPIC dialog box:
3.
Click Load In Select From Library dialog box:
Highlight “AISI 4340 Steel” from the selection list
Notice: Any material properties entered manually by the user can be saved in the library and recalled for future use by giving the material a name and clicking the save button in the Define Material - ISOTROPIC dialog box. To place the material in a new model, click the Load button, select it from the list and click OK.
Creating the Materials and Properties
4.
26-3
Click OK, then…
In Define Material - ISOTROPIC dialog box:
Click OK, then…
Click Cancel What Create the tubular Beam Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Beam radio button in Line Elements section Click OK
5.
In Define Property – BEAM Element Type dialog box:
6.
Type “Square Tube” in Title field Select “AISI 4340 Steel” from the Material drop down menu
7.
Click Shape button
8.
In Cross Section Definition dialog box:
Select “Rectangular Tube” from the Shape drop down menu
26-4 9.
Gap Contact - Cantilever Beam
Enter the following values into the corresponding fields in the Size section of the dialog box:
Height = 0.5
Width = 0.5
Thickness = 0.1
Click the Draw Section Button to see the defined section
10.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Curves
What Set the mesh size on the curves
Creating the Materials and Properties
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Size Along Curve
Menu
2.
Entity Selection – Select Curve(s) to Set Mesh Size
Choose the curve (curve 1) 3.
Click OK
4.
In Mesh Size Along Curves dialog box:
5.
Enter “10” in Number of Elements field Click OK, then…
Click Cancel
What Mesh the line
How Step 1.
UI
Command/Display Mesh, Geometry, Curve
Menu
2.
Entity Selection – Select Curve(s) to Mesh
Choose curve 1 3.
Click OK
4.
In Geometry Mesh Options dialog box:
5.
Select “Square Tube” from the Property drop down menu Click OK
6.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 1, Z = 0
26-5
26-6
Gap Contact - Cantilever Beam
7. 8.
Click OK, then… Crtl-Q
This will bring up the View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 9.
Click Geometry Off button, then…
Click Done
Creating the Gap property and element Every Gap element MUST have a Gap property associated with it that has the correct Initial Gap distance value. Compression and Tension Stiffness values are also required to control the closing of the “gap”. In this example, only one gap element is required, therefore only one Gap Property must be created. If a model would require multiple Gap elements to be created at a number of different initial gap distances, then an individual Gap Property must be created for EVERY different initial gap distance. Gap Contact is a node-to-node method of contact and therefore should have a corresponding number and spacing of nodes on each contact line or surface for effective convergence of the Nonlinear Analysis.
What Create a Node to represent the other side of the “Gap”
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Curser dialog box:
3.
Enter: X = 7, Y = -0.5, Z = 0, Click OK, then…
Click Cancel
What Create a Gap Property
How
Creating the Gap property and element
Step 1.
UI
26-7
Command/Display Model, Property
Menu
2.
In Define Property – BEAM Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Gap radio button in Line Elements section Click OK
5.
In Define Property – GAP Element Type dialog box:
Type “Gap” in Title field
Enter “0.5” in Initial Gap field
Enter “1000000” in Compression Stiffness field
Enter “0.0001” in Tension Stiffness field
Notice: A great way to determine the Initial Gap value for a gap of undetermined distance is to use the “Distance Measurement Tool” in FEMAP. This can be accessed by highlighting the Initial Gap field (or any other dialog box field which requires a distance) and pressing Ctrl-D on the keyboard. This will bring up a “point-to-point” measuring tool prompting the user to choose a start point, clicking OK, then prompting for an end point and clicking OK. This is a very helpful FEMAP tool.
26-8 6.
Gap Contact - Cantilever Beam
Click OK, then…
Click Cancel What Create a Gap element between a node on the beam and the newly created node
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define GAP Element – Enter Nodes or Select with Cursor dialog box:
Choose the 8th node from the left side of the beam (Node 8) and the newly created node (Node 12)
Node 8
Node 12
3.
Click Vector button
4.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 5.
Tip X = 0, Y = 0, Z = 1 Click OK
6.
In Define GAP Element – Enter Nodes or Select with Cursor dialog box:
Select “Gap” from the Property drop down menu
Creating the loads and constraints
7.
Click OK, then…
Click Cancel
Creating the loads and constraints What Apply a fixed constraint to the left end of the beam and the “bottom node” of the Gap
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
26-9
26-10 5.
Gap Contact - Cantilever Beam
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the fixed end of the beam (Nodes 1) and the node on the “bottom” of the gap (node 12)
Node 1
Node 12
6.
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Apply a Force to the free end of the beam
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Force” in the Title field Click OK
Creating Settings for Nonlinear analysis
4.
26-11
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the beam (Node 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “-2000” in FY field (units: Pounds)
9.
Click OK, then…
Click Cancel The model should now look like this:
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the
26-12
Gap Contact - Cantilever Beam
steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX Nastran through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
Running the Nonlinear Static Analysis
26-13
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Gap Contact” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
26-14
Gap Contact - Cantilever Beam
Post-Processing the Gap Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation results of the beams is with a deformed plot. The best ways to view the stress results on the beam is with the Beam Diagram contour capability.
What View the results in a FEMAP Beam Diagram plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Beam Diagram radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “10..Case 10 Time 1.” from drop down menu located in the Output Set section, then…
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
5.
Select “3139..Beam EndA Pt1 Comb Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
In View Select dialog box:
Click OK
Post-Processing the Gap Contact Results
6.
26-15
Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting PostProcessing as the Category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Command Toolbar for this task View, Options or…
7. Menu
8.
9.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “Beam Diagram” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “3..Global Y” from the Default Direction selection list
26-16
10.
Gap Contact - Cantilever Beam
Click OK
The Beam Diagram plot of the deformed model should look like this:
This Concludes the Gap Contact example. It is recommended to save the model file.
Large Deformation - Cantilever Beam 27.
Nonlinear Analysis is analysis which often consists of models which undergo large deformations due to geometric or material nonlinearities. This realm of analysis includes such other concepts as plastic deformation, snap-through, creep, physical contact between objects, shrink-fitting, hyperelastic materials, and thin-shell buckling. The behavior experienced by many objects and systems in the world can be modeled with a greater degree of accuracy using the nonlinear capabilities of NX Nastran.
Two separate cantilever beams with I-Beam Cross Sections will be used to demonstrate large deformations usually found in Nonlinear Static Analysis. For the beam properties one Standard Cross Section (PBEAM) and one NASTRAN Beam (PBEAML) will be created. The beams will have one end fixed, and the free end will be loaded with a Moment. This example will use the Nonlinear Static solving capability of NX/Nastran.
For this example a beam model will be created using FEMAP. The analysis process includes:
· creating a beam property two separate ways, mesh an existing curves, and viewing the cross-sections of the elements
· creating Moment loads on free ends of I-Beams and fixed constraints
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the large deformations of I-Beams using FEMAP’s Multi-Set Animation capability
Creating the Geometry What Create lines to represent the beams
How
Step 1.
UI Menu
Command/Display File, New
27-2 2.
Large Deformation - Cantilever Beam
Geometry, Curve-Line, Coordinates Menu
3.
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 300, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 200, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
4.
X = 300, Y = 0, Z = 200 Click OK, then
5.
Click Cancel View, Rotate, Model or… Menu
Press the F8 Key 6.
In View Rotate dialog box:
Click Isometric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
Creating the Materials and Properties
27-3
Creating the Materials and Properties What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
In Define Material - ISOTROPIC dialog box:
Type “I-Beam” in Title field, then…
Enter “200,000” in Young’s Modulus, E field (units: N/mm2)
Enter “0.3” in Poisson’s Ratio, nu field Click OK, then…
3.
Click Cancel
FEMAP has two separate ways to define the cross section of a beam property. Both methods allow the user to pick from a list of “pre-defined cross sections” and enter in specific values for the dimensions. The Standard Beams (PBEAM) also allow the user to create a General Section (choose from any planer surface), choose the stress recovery points, define the orientation of the Y-axis on the property form, and choose to calculate the Shear Center offset and Warping Constant. The NASTRAN Beam (PBEAML) allows changes to the dimension of the beam on the actual PBEAML property input card and always calculates the Shear Center offset and Warping Constant. Both Beams use the Cross Section Y-axis for orientation, but the relationship between the Cross section Y-Axis and Z-Axis are opposite for the two types of beams
What Create the Standard Beam Property
How
Step 1.
UI Menu
Command/Display Model, Property
27-4
Large Deformation - Cantilever Beam
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Beam radio button in Line Elements section Click OK
5.
In Define Property – BEAM Element Type dialog box:
6.
Type “Standard Beam” in Title field Select “I-Beam” from the Material drop down menu
7.
Click Shape button
8.
In Cross Section Definition dialog box:
9.
Select “I-Beam or Wide Flange (W)” from the Shape drop down menu Enter the following values into the corresponding fields in the Size section of the dialog box:
Height = 8 Width, Top = 8 Width, Bottom = 8 Thick, Top = 0.5 Thick, Bottom = 0.5 Thickness = 0.5 (this is the thickness of the web of the beam)
Click the Draw Section Button to see the defined section Notice: If you choose the “Compute Warping Constant” option when creating a beam cross-section (not used in this example), FEMAP will calculate the warping constant for the cross section. FEMAP bring up this message box when the model using this option is exported for analysis:
Simply click Yes to use the “scalar points” created by FEMAP for post-processing.
Creating the Materials and Properties
10.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel What Create the NASTRAN Cross Section Beam Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – BEAM Element Type dialog box:
Type “NASTRAN Beam” in Title field
27-5
27-6
Large Deformation - Cantilever Beam
3.
Select “I-Beam” from the Material drop down menu
4.
Click Shape button
5.
In Cross Section Definition dialog box:
6.
Choose NASTRAN radio button in upper right corner of dialog box Select “NASTRAN I” from the Shape drop down menu
7.
Enter the following values into the corresponding fields in the Size section of the dialog box:
DIM1 = 8 (Height) DIM2 = 8 (Width, Bottom) DIM3 = 8 (Width, Top) DIM4 = 0.5 (thickness of the web of the I-beam) DIM5 = 0.5 (Thick, Bottom) DIM6 = 0.5 (Thick, Top) Click the Draw Section button to see the defined section Notice: It is very important to hit the Draw Section button, especially with the ambiguity of the dimension (DIM) values when creating the NASTRAN beams to make sure the beam dimensions are accurate.
Creating the Materials and Properties
8.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Curves
What Set the mesh size on the curves
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Size Along Curve
Menu
2.
Entity Selection – Select Curve(s) to Set Mesh Size
Choose both curves (curve 1 and 2) 3.
Click OK
4.
In Mesh Size Along Curves dialog box:
5.
Enter “15” in Number of Elements field Click OK, then…
Click Cancel
What Mesh the line
How
Step
UI
Command/Display
27-7
27-8 1.
Large Deformation - Cantilever Beam
Mesh, Geometry, Curve Menu
2.
Entity Selection – Select Curve(s) to Mesh
Choose curve 1
Curve 1
Curve 2
3.
Click OK
4.
In Geometry Mesh Options dialog box:
5.
Select “Standard Beam” from the Property drop down menu Click OK
6.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 0, Z = 1 Click OK
7. 8.
Mesh, Geometry, Curve Menu
9.
Entity Selection – Select Curve(s) to Mesh
Choose curve 2 10.
Click OK
Creating the Materials and Properties
11.
In Geometry Mesh Options dialog box:
12.
Select “NASTRAN Beam” from the Property drop down menu Click OK
13.
In the Vector Locate – Define Element Orientation Vector dialog box:
27-9
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 1, Z = 0
Notice: This is a different orientation vector than was used with the standard beam Property Click OK
14. 15.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 16.
Click Geometry Off button, then…
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. Viewing the Beam Cross Sections
What Utilize the View Options to visualize Beam Cross Sections
How
Step 1.
UI
Command/Display View, Options or…
Menu
Press the F6 Key or choose “Options” from the View Style icon
on the View Toolbar
27-10
Large Deformation - Cantilever Beam
2.
In View Options dialog box:
3.
Choose Entities, Labels, and Colors radio button under Category Highlight “Element – Orientation/Shape” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “3..Show Cross Section” from the Element Shape selection list Click OK
4.
Tip: You can also “toggle” the cross-sections of line elements on/off using the “Thickness/Cross Section” command from the View Style menu located on the View Toolbar. The model should now look like this:
Fixed End
Free End
Creating the loads and constraints What Apply fixed constraints to the fixed end of both beams How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating the loads and constraints
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the node at the fixed end of each beam (Nodes 1 and 17) 6.
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Apply a moment to the free end of each beam
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Moment” in the Title field Click OK
4.
Model, Load, Nodal Menu
27-11
27-12 5.
Large Deformation - Cantilever Beam
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of each beam (Nodes 16 and 32) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Moment from the selection list 8.
Enter “534000” in MZ field (units: Nmm)
9.
Click OK, then…
Click Cancel
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX Nastran through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis.
Running the Nonlinear Static Analysis
27-13
4.
Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
27-14
Large Deformation - Cantilever Beam
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Large Deformation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Large Deformation Results The Nonlinear Static Analysis has been completed. The best way to view the deformation results of the beams is with a deformed plot.
What View the deformation results in a FEMAP deformed plot
How
Step
UI
Command/Display
Post-Processing the Large Deformation Results
1.
27-15
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Deform radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “Last Analysis Step, Time 1” (Should be Step 21, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in Output Vectors section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting Postprocessing as the Category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Post Options menu on the Post Toolbar for this task
27-16
Large Deformation - Cantilever Beam
The Post Options icon
also has these toggles and options
1. Undeformed: Turn the Undeformed Model On and Off 2. Scale Deformation: Set a Deformation Scale for the Model 3. Animation Frames: Set the number of frames used in Animation 4. Animation – Positive Only: Animate only in the loaded direction 5. Animation – Load and Unload: Animate loading only, then repeat 6. Animate Contours: Animate the contours as the model deforms 7. Filled Contours: Use outlines only for contours 8. Contour Options…: Bring up the Contour Options dialog box 9. Freebody...: Bring up the View Freebody Options dialog box 10. More options…: Bring up the View Options dialog box
Most of these options relate to Animation of one Output Set only. View, Autoscale, Visible
7. Menu
OR Press Ctrl - A The deformed plot of the nodal displacements actual deformation should look like this:
If you would like to toggle the “Undeformed” model on and off to compare the deformed model to the original model, click the Post Options icon on the Post Toolbar and select Undeformed from the drop down list. Animating the Results Using Animate Multi-Set
What View all the Output Sets in one sequential animation
How Step
UI
Command/Display
Post-Processing the Large Deformation Results
1.
27-17
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate-MultiSet radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
Select “1..Case 1 Time 0.05” from Output Set drop down menu
Select “21..Case 21 Time 1” from Final Output Set drop down menu Click OK
5.
In Selecting PostProcessing Data dialog box:
Click OK, then…
In View Select dialog box:
Click OK Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The model should now be animating the deformations one step at a time.
Use the View, Advanced Post, Animation menu command to speed up and slow down the animation.
What Return the model to a deformed plot
How Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
27-18
Large Deformation - Cantilever Beam
2.
In View Select dialog box:
3.
Choose Deformed radio button in Deformed Style section Click OK
This Concludes the Large Deformation example. It is recommended to save the model file.
Slide Line Contact - Hyperelastic Seals 28.
Two semicircular seals are being pressed together at a given enforced displacement. The seals are the same size and shape and the rounded sides of the seals will come into contact with one another. The seals are made of a hyperelastic material and the model allows the use of plane strain elements for analysis. Contact between the rounded sides of each seal will be modeled using Slide Line Contact. Slide line contact differs from Gap contact in that is not simply a point-to-point or nodeto-node representation of contact, but a 2-D relationship between a set of Master nodes and a set of Slave Nodes. This example will use the Nonlinear Static solving capability of NX Nastran.
For this example a model of two seals has already been created. The analysis process includes:
· modifying the hyperelastic material
· creating a Slide Line property and then selecting the Master and Slave sets to create the slide line element for contact
· creating an Enforced Displacement to bring the seals together into contact
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the multi-set animation of the analysis sets to understand how the contact between the seals progresses
Upper Seal
Lower Seal
28-2
Slide Line Contact - Hyperelastic Seals
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Nonlinear/seals.neu Locate seals.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Modifying the Material
28-3
Modifying the Material The seals need to be made of a hyperelastic material. The model currently has an isotropic material defined. The type of material needs to be selected and the correct Directional and Volumetric Deformation Constants entered for the analysis to run correctly.
What Modify the Material
How
Step 1.
UI
Command/Display Modify, Edit, Material
Menu
2.
In Entity Selection – Select Material(s) to Edit dialog box:
Click OK, then…
In Define Material - ISOTROPIC dialog box:
3.
Click Type button Tip: You can also edit an existing Material using the Edit command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight any existing Material, then right mouse click to see the context sensitive menu). In Material Type dialog box:
4.
Choose Hyperelastic radio button Click OK
5.
In Define Hyperelastic Material dialog box: Type “Hyperelastic” in Title field Enter “100” in Table10 (A10) field in Directional Deformation Constants (Aij) section Enter “0.005” in Table01 (A01) field in Directional Deformation Constants (Aij) section Enter “10000” in first Volumetric Deformation Constants (Di) field
28-4
6.
Slide Line Contact - Hyperelastic Seals
Click OK
Creating the Slide Line Property and Element The Slide Line Element requires a property be defined to include values for Master width, Slave width, Non-Sliding Frictional Stiffness, Static Friction Coefficient and Stiffness Scale Factor. Additionally, the Slide Line Plane can be defined, as well as, a check to specify Unsymmetrical or Symmetrical Penetration.
Here are some additional considerations that should be taken into account when using Slide Line Contact:
· Slide Line Contact must always be used in conjunction with Static or Transient Nonlinear Analysis.
· The XY Plane for Slide Line Contact is always defined by the global or local coordinate system that is referenced in the Slide Line property.
· Master and Slave designation is for naming purposes only in symmetric penetration. When Unsymmetrical Penetration is used, only Slave nodes are checked for penetration into the Master segment
· The Z-axis of the reference coordinate system in the Slide Line Property is used to align the slide line elements. The right hand rule should be taken into account when selecting Master and Slave nodes. Slave and Master segment Normals MUST face each other.
Creating the Slide Line Property and Element
28-5
· When performing Static Nonlinear analysis, try to use an enforced displacement instead of applied loads, if possible, due to better convergence of the model. (Enforced displacement can not be used in Transient Nonlinear Analysis)
What Create the Slide Line Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property Type button In Element / Property Type dialog box:
4.
Choose Slide Line radio button in Other Elements section Click OK
5.
In Define Property – SLIDE LINE Element Type dialog box:
Type “Slide Line” in Title field Enter “1.95” in Master Width field Enter “1.95” in Slave Width field Enter “0.5” in Nonsliding Frictional Stiffness field Enter “0.4” in Static Friction Coefficient field
Notice: The slide line plane used in this analysis in the 0..Basic Rectangular, but a local coordinate system could be generated and referenced for a slide line that does not lie in the Global XY Plane.
Notice: Symmetrical Penetration is often more accurate when contact is occurring between two bodies which allow the same level of penetration, but creates longer computation times than Unsymmetrical Penetration.
28-6
6.
Slide Line Contact - Hyperelastic Seals
Click OK, then…
Click Cancel What Create the Slide Line Element
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
3.
Select “Slide Line” from the Property drop down menu Click Master Nodes button
Creating the Slide Line Property and Element
4.
28-7
Entity Selection – Select Master Nodes
Choose nodes on the lower seal in the following order: (Nodes 183 to 189 and Nodes 254 to 261)
Start Here
5.
End Here
Notice: It is critical to choose the nodes one at a time, in this order for the Slide Line Element to work properly Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click Slave Nodes button
28-8 6.
Slide Line Contact - Hyperelastic Seals
Entity Selection – Select Slave Nodes
Choose nodes on the Upper seal in the following order: (Nodes 100 to 106 and Nodes 6 to 13)
End Here
Start Here
Notice: It is recommended to choose the Slave nodes one at a time, in the reverse order of the Master nodes for the Slide Line Element to work more effectively Click OK
7.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click OK, then…
Click Cancel
Creating the loads and constraints What Apply constraints to the bottom of the Lower Seal to not allow translation in the Y and Z directions, and “fix” the center node in the X-direction as well.
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating the loads and constraints
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the bottom of the Lower Seal using a box pick:
Node 167 6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY and TZ boxes Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Center node at the bottom of the Lower Seal (Node 167) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
CHECK TX, TY, and TZ boxes
28-9
28-10 12.
Slide Line Contact - Hyperelastic Seals
Click OK, then…
In NX Nastran for FEMAP dialog box:
“Selected Constraints Already Exist. OK to Overwrite (No=Combine)?”
Click Yes, then…
Click Cancel What Apply Enforced Displacements to the top of the Upper Seal
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Displacements” in the Title field Click OK
4.
Model, Load, Nodal Menu
Creating the loads and constraints
5.
28-11
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the top of the Upper Seal using a box pick:
6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 8.
Enter “-0.6” in TY field (units: Inches)
9.
Click OK, then…
Click Cancel What Apply constraints to the top of the Upper Seal to not allow translation in the Z direction, and “fix” the center node in the Xdirection as well. Also, in NX Nastran, the degree of freedom in the direction of an Enforced Displacement must be constrained. Therefore, the Y-translation of all the nodes on the top of the Upper seal must be constrained.
How
Step 1.
UI Menu
Command/Display Model, Constraint, Nodal
28-12 2.
Slide Line Contact - Hyperelastic Seals
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the top of the Upper Seal using a box pick:
Node 1
3.
Click OK
4.
In Create Nodal Constraints/DOF dialog box:
5.
CHECK TY and TZ boxes Click OK
6.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Center node at the bottom of the Lower Seal (Node 1) 7.
Click OK
8.
In Create Nodal Constraints/DOF dialog box:
9.
CHECK TX, TY, and TZ boxes Click OK, then…
In NX Nastran for FEMAP dialog box:
“Selected Constraints Already Exist. OK to Overwrite (No=Combine)?”
Click Yes, then…
Click Cancel
Creating Settings for Nonlinear analysis
28-13
The Model should now look like this:
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX NASTRAN through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
Choose Static radio button
28-14
Slide Line Contact - Hyperelastic Seals
3.
Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “30” into Number of Increments field
5.
Notice: Contact Analysis often requires a higher number of increments to improve convergence of a solution. Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
Post-Processing the Slide Line Contact Results
28-15
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Slide Line” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Slide Line Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the seals is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What
28-16
Slide Line Contact - Hyperelastic Seals
View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon In View Select dialog box:
2.
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 37, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “7233..Plate Mid VonMises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Post-Processing the Slide Line Contact Results
28-17
The deformation and stress results should look like this:
Zoom in on the Contact Region:
The Nodes do no meet up exactly as in gap contact because they are allowed to slide along the Slide Line as the model changes shape.
What View the results in a FEMAP Animation of all the analysis sets
28-18
Slide Line Contact - Hyperelastic Seals
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.0333333)” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 37, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model
The Contact between the seals can be viewed in this mode as the seals are pushed together.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This Concludes the Slide Line Contact example. It is recommended to save the model file.
3-D Contact - Plastic Clip and Base 29.
A plastic clip made of solid elements will come into contact with a fixed base and move through a range of motion based on enforced displacements using slide line contact.
For this example the clip and the base have already been created. The analysis process includes:
· creating Slide Line elements by selecting the Master and Slave node sets for contact
· creating an Enforced Displacement to bring the Clip into contact with the Base
· defining the analysis parameters to aid in convergence of the Nonlinear solution
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the multi-set animation of the analysis sets to understand the contact between the objects.
Plastic Clip
Fixed Base
29-2
3-D Contact - Plastic Clip and Base
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Nonlinear/snapfit.neu Locate snapfit.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are solid 3-D elements.
Creating the Contact (Slide Line) Element
29-3
Creating the Contact (Slide Line) Element What Create the Slide Line Element
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define PLATE Elements – Enter Nodes or Select with Cursor dialog box:
3.
Click Type button In Element / Property Type dialog box:
4.
Choose Slide Line radio button in Other Elements section Click OK
5.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
6.
Select “Slide Line” from the Property drop down menu Click Master Nodes button
7.
In Entity Selection – Select Master Nodes dialog box:
Click Pick button, then select Front from the menu
Notice: This will allow the user to choose the entity that is in front of other entities. The screen is always the XY plane in this command, so the entity that is in the “front” is the entity that has the highest value in the “Z-direction” (perpendicular to the XY plane of the screen).
29-4 8.
3-D Contact - Plastic Clip and Base
Choose nodes on the fixed base in the following order: (Nodes 1145 to 1179)
End Here
Start Here
9.
Notice: It is critical to choose the nodes one at a time, in this order for the Slide Line Element to work properly. Also, be sure that only one node is chosen at each location, the slide line property specifies the XY Plane used and any nodes chosen outside that plane will cause the analysis to end without running. Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
10.
Click Slave Nodes button Entity Selection – Select Slave Nodes Choose nodes on the Plastic Clip in the following order: (Nodes 30 to 31, 557-571, 422-435, and Node 53)
Start Here
End Here
Notice: It is recommended to choose the Slave nodes one at a time, in the reverse order of the Master nodes for the Slide Line Element to work more effectively
Creating the Contact (Slide Line) Element
11.
29-5
Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click OK, then…
In NX Nastran for FEMAP dialog box:
Click NO (The elements were selected in the correct order, so the selection order does not need to be reversed), then...
Click Cancel The Model should now look like this:
Creating the permanent constraints
For this example every node will have some degrees of freedom permanently constrained in order for the analysis to run correctly and more efficiently. For example the base will be fixed for the duration of the analysis and is assumed to be undeformable. Therefore, all the nodes of the base will be permanently constrained. Because of this, stress values will only be calculated for the plastic clip.
What Create Permanent Constraints on multiple nodes with one command.
How
29-6
Step 1.
UI
3-D Contact - Plastic Clip and Base
Command/Display Modify, Update Other, Perm Constraint
Menu
2.
In Entity Selection – Select Node(s) to Update Permanent Constraints dialog box:
Click Select All, then…
3.
Click OK In Update Nodal Permanent Constraints dialog box:
CHECK TZ, RX, and RY boxes
4.
Click OK
5.
In Entity Selection – Select Node(s) to Update Permanent Constraints dialog box:
Choose all the nodes of the fixed base with a box pick (Hold Shift and drag a box around the fixed base)
Creating the loads and constraints
6.
29-7
In Update Nodal Permanent Constraints dialog box:
CHECK TX, TY, TZ, RX, RY and RZ boxes
7.
Click OK
Creating the loads and constraints What Apply constraints to the bottom of the Clip to not allow translation in the Y direction, and “fix” the loaded nodes in the X Translation direction as well. In order for NX Nastran to use enforced displacements, the degree of freedom in the direction of the enforced displacement must be constrained.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
29-8 5.
3-D Contact - Plastic Clip and Base
Entity Selection – Enter Node(s) to Select dialog box:
Select the 6 nodes shown at the bottom of the Clip using a box pick: (Nodes 74-76 and 730-732)
Nodes to be constrained in TY
6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY box Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Nodes to be constrained in TX and TY
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
12.
CHECK TX and TY boxes Click OK, then…
Click Cancel What Apply Enforced Displacements to the nodes constrained in both X and Y Translation in the step above (nodes 73 and 729)
How
Step
UI
Command/Display
Creating Settings for Nonlinear analysis
1.
29-9
Model, Load, Set Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Displacements” in the Title field Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 8.
Enter “2.25” in TX field (units: Inches)
9.
Click OK, then…
Click Cancel
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. For this Nonlinear Static analysis the number of increments will be set to a larger number than many of the previous examples in order to aid solution convergence.
What Create Nonlinear Static settings
How
Step 1.
UI Menu
Command/Display Model, Load, Nonlinear Analysis
29-10
3-D Contact - Plastic Clip and Base
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Enter “75” into Number of Increments field
5.
Notice: Contact Analysis often requires a higher number of increments to improve convergence of a solution. Select “1..Yes” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
Post-Processing the Slide Line Contact Results
29-11
How Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Snapfit” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Slide Line Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multiset Animation.
What View the results in a FEMAP contour plot of a deformed model
29-12
3-D Contact - Plastic Clip and Base
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon In View Select dialog box:
2.
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 83, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “60031..Solid Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Post-Processing the Slide Line Contact Results
29-13
The deformation and stress results should look like this:
What View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.0333333)” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 83, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically.
29-14 5.
3-D Contact - Plastic Clip and Base
Click OK, then…
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The Contact between the Clip and the Base can be viewed in this mode as the objects come into contact.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the 3-D Contact example. It is recommended to save the model file.
Large Deformation - Advanced Nonlinear (SOL 601) 30.
A small part made of plate elements will be subjected to a functionally-dependent load and experience large deformation.
For this example the part already been created. The analysis process includes:
· creating a functionally-dependent Load to create large deformation.
· defining the analysis parameters for the Nonlinear solution (Analysis Set Manager)
· analyzing the model with NX Nastran’s Advanced Nonlinear Solution (SOL 601)
· viewing the deformed plot and multi-set animation of the analysis sets to see the large deformation.
Part
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, Materials, and Constraints
30-2
Large Deformation - Advanced Nonlinear (SOL 601)
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Advanced_Nonlinear/Large601.neu Locate Large601.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are Plate Elements. The nodes at the bottom edge of the part are fixed in all degrees of freedom.
Creating the functionally dependent loads
30-3
Creating the functionally dependent loads What Apply functionally dependent Forces to nodes opposite the constrained edge in the positive Z direction. The function will be used to “step” the load up as the analysis progresses.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Loading Function” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Linear Ramp radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 1 Delta X = 0.05 Y = 0.0 To Y = 1
30-4 6.
Large Deformation - Advanced Nonlinear (SOL 601)
Click More button
X and Y Values will be created for the function.
7.
Note: This will produce values from 0 to 0.95. A final data point will be added to insure the load has been fully applied. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X =1.0 Y = 1.0 Click OK, then…
10.
Click Cancel Model, Load, Set Menu
11.
In Create or Activate Load Set dialog box:
12.
Type “Forces” in the Title field Click OK
13.
Model, Load, Nodal Menu
14.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 3 nodes on the edge opposite the constrained edge (Nodes 55, 56, and 57).
Running the Nonlinear Static Analysis
15.
Click OK
16.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 17.
Enter “1333.3” in FZ field
18.
Select “1..Loading Function” from Time/Freq Dependence drop down menu.
19.
Click OK, then…
Click Cancel The Model should now look like this:
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Advanced Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
30-5
30-6 1.
Large Deformation - Advanced Nonlinear (SOL 601)
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Large 601” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “22..Advanced Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next button 2 times
6.
In NASTRAN Bulk Data Options dialog box:
CHECK LGDISP box
7.
Note: This PARAM in NX Nastran is very important for Large Displacement Analysis. Without the PARAM answers will be considerably different and inaccurate. Click Next button 3 times
8.
In NXSTRAT Solver Parameters dialog box
Enter “20” in the Number of Steps field in the Time Steps section
Enter “0.05” in the Time Increment field in the Time Steps section
Running the Nonlinear Static Analysis
9.
Click Next button 1 time
10.
In NXSTRAT Iteration and Convergence Parameters dialog box
30-7
Select “1..On” from the Auto Increment drop down menu in the Analysis Control section.
30-8
11.
Large Deformation - Advanced Nonlinear (SOL 601)
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Large Deformation Results The Advanced Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Post-Processing the Large Deformation Results
2.
30-9
In View Select dialog box:
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “20..Case 20 Time 1.” (Should be Step 20, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “7033..Plate Top Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the Post Toolbar and select Actual Deformation from the drop down list (Must have a check mark next to it in the menu)
7.
Ctrl+A
Ctrl+A will perform the View, Autoscale, Visible command.
Note: Use the magnify down icon on the View Toolbar or spin the wheel of a wheel mouse until the entire deformed image can be seen.
30-10
Large Deformation - Advanced Nonlinear (SOL 601)
The deformation and stress results should look like this:
What
View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
Post-Processing the Large Deformation Results
4.
30-11
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.01)” from drop down menu located in the Output Set section
Select “20..Case 20 Time 1.” (Should be 20, but may differ based on machine set-up) from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The part can now be viewed as it experiences large deformation.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the Large Deformation - Advanced Nonlinear (SOL 601) example. It is recommended to save the model file.
30-12
Large Deformation - Advanced Nonlinear (SOL 601)
Surface to Surface Contact Advanced Nonlinear (SOL 601) 31.
A clip made of solid elements will come into contact with a fixed base and move through a range of motion based on enforced displacements using surface to surface contact.
For this example the clip and the base have already been created. Also, permanent constraints and the contact segments have also been created to focus the example on performing the analysis. The analysis process includes:
· creating the Connection Property and defining the Connector for surface to surface contact in NX Nastran.
· creating a functionally-dependent Enforced Displacement to bring the Clip into contact with the Base
· defining the analysis parameters to aid in convergence of the Nonlinear solution (Analysis Set manger)
· analyzing the model with NX Nastran’s Advanced Nonlinear Solution (SOL 601)
· viewing the multi-set animation of the analysis sets to understand the contact between the objects.
Plastic Clip
Base
31-2
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, Materials, Permanent Constraints, and Connection Regions
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Advanced_Nonlinear/snap601.neu Locate snap601.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are solid 3-D elements.
Creating the Contact Conditions
31-3
Creating the Contact Conditions In order for surface to surface contact to occur during analysis with NX Nastran Advanced Nonlinear Method (SOL 601), several parameters must be defined. In general, Connection Regions are created, a Connection Property is defined, and then a Connector (“contact pair”) is created to define the contact relationship between the two Connection Regions. First, Connection Regions must be created using the Connect, Connection Region command. While this dialog box is open, elements and element faces can be chosen to represent the areas on different parts in the model that will come into contact with one another. The process consists of choosing all elements around the outside edge of a part that may possibly come into contact with another part. Once these elements are chosen, an element face must be chosen to allow NX Nastran to know what face of the element will be part of a contact surface. When all the elements have be chosen and faces selected, the Connection Region will, by default, be shown as orange colored “plate elements” with thick orange edges on the screen. For this model, the Connection Regions have been created to save modeling time and focus on the use of the NX Nastran Advanced Nonlinear solution sequence (SOL 601). Viewing the Connection Regions will show how these regions should be created. The regions in this model were created by choosing the Elements radio button then clicking the Multiple button in the Define Connection Region dialog box. Multiple allows a number of elements around the edge of the part to be chosen at the same time, then element faces are selected using the Adjacent Faces option in the Face Selection for Elemental Loads dialog box. What Viewing the Connection Regions
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
In View Quick Options dialog box:
3.
Click All Entities Off button CHECK Connection Region box located in the Others section, then...
4.
Click Done
This will make only the contact segments visible on the screen. These segments will be used along with a contact property to create a contact pair to be used for surface to surface contact. Rotate the View to be able to see the element faces which make up the contact segments.
Deformable
Rigid
31-4
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
After the Connection Regions have been created and visually confirmed, the next step in creating a Connector (contact pair) is creating the Connection Property. Because this type of property is unique, it will only be found as command on the Connect menu. There are three type of contact used by SOL 601 which FEMAP supports: Constraint Function, Segment Method, or Rigid Target. Along with each type of contact there a number of parameters which can be set to define the behavior of the parts that will come into contact. The contact type is usually determined by the type of problem trying to be solved. Also, birth time and death time for a Connection Regions can be defined. For more information on the options see Section 4.4 Creating Connections (NX Nastran Contact Properties) of the FEMAP Commands manual or the Theory and Modeling guide of SOL 601. In this case, the Constraint Function type of contact will be used with the default values assigned.
What Create the Connection Property
How
Step 1.
UI
Command/Display Connect, Connection Property
Menu
2.
Tip: You can also create a new Connection Property using the New command on the “context sensitive menu” located on the Connection Property branch in the Model Info tree (simply click to highlight the top level of the Connection Properties branch or any existing Connection Property, then right mouse click to see the context sensitive menu). In Define Connection Property dialog box:
Type “Contact” in the Title field 3.
Click the NX Adv Nonlin tab in the Define Connection Property dialog box
4.
Make sure that “0..Constraint Function” is selected from the Contact Type drop down menu in the General section.
5.
Also, make sure that Connect Type is set to “0..Contact” (This drop-down is located in the upper right corner of the Define Connection Property dialog box) Click OK, then...
Click Cancel Finally, once the Connection Property has been defined, the Connector (contact pair) can be created. In order to create a Connector, a “Master” Connection Region and a “Slave” Connection Region must be chosen from available Connection Regions. In this model, the Connector will be created to minimize convergence time during the solution. What Create the Connector (contact pair)
Creating the Contact Conditions
31-5
How
Step 1.
UI
Command/Display Connect, Connector...
Menu
2.
In the Define Contact Connector - Select Connection Regions dialog box:
Choose “1..Contact” from the Property drop-down list.
Choose “1..Deformable” from the Master drop-down list.
Choose “2..Rigid” from the Slave drop-down list. Click OK
3. 4.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 5.
CHECK Element box located in the Others section, then
6.
Click Load/Constraint On
Click Done
7.
Crtl-R
This will show the elements and contact segments only. A single line element will be shown from contact segment to contact segment to represent a contact pair exists between the segments. This will bring up View Rotate dialog box:
OR F8 key 8.
Click XY Top, then...
Click OK Tip: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
31-6
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
The Model should now look like this:
Creating the loads and constraints What Apply constraints to the bottom of the Clip to not allow translation in the Y direction, and “fix” the nodes which will be loaded with the functionally-dependent Enforced Displacement in the X-direction as well.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Tip: You can also create a new Constraint Set using the New command on the “context sensitive menu” located on the Constraints branch in the Model Info tree (simply click to highlight the top level of the Constraints branch or any existing Constraint Set, then right mouse click to see the context sensitive menu). Model, Constraint, Nodal Menu
Creating the loads and constraints
5.
31-7
Entity Selection – Enter Node(s) to Select dialog box:
Select the 6 nodes shown at the bottom of the Clip using a box pick: (Nodes 74-76 and 730-732)
Nodes to be constrained in TY
6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY box Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Nodes to be constrained in TX and TY
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
12.
CHECK TX and TY boxes Click OK, then…
Click Cancel What Apply functionally dependant Enforced Displacements to the nodes constrained in both the X and Y Translation directions in the last step. The function will be used to “step” the displacement load up as the analysis progresses.
How
Step
UI
Command/Display
31-8 1.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
Model, Function Menu
2.
In Function Definition dialog box:
3.
Type “Loading function” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Linear Ramp radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 1 Delta X = 0.01 Y = 0.0 To Y = 1 6.
Click More button
X and Y Values will be created for the function.
7.
Note: This will produce values from 0 to 0.99. A final data point will be added to insure the load has been fully applied. Choose Single Value radio button
Running the Nonlinear Static Analysis
8.
Enter the following values in the corresponding fields:
9.
X =1.0 Y = 1.0 Click OK, then…
10.
Click Cancel Model, Load, Set Menu
11.
In Create or Activate Load Set dialog box:
12.
Type “Displacements” in the Title field Click OK
13.
Model, Load, Nodal Menu
14.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 15.
Click OK
16.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 17.
Enter “2.25” in TX field (units: Inches)
18.
Select “1..Loading Function” from Time/Freq Dependence drop down menu.
19.
Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Advanced Nonlinear Static Analysis using the FEMAP Analysis Set Manager
31-9
31-10
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Snapfit 601” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “22..Advanced Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next button 2 times
6.
In NASTRAN Bulk Data Options dialog box:
7.
CHECK LGDISP box Click Next button 3 times
8.
In NXSTRAT Solver Parameters dialog box
Enter “100” in the Number of Steps field in the Time Steps section
9.
Enter “0.01” in the Time Increment field in the Time Steps section Click Next button 1 time
Post-Processing the Surface to Surface Contact Results
31-11
10.
In NXSTRAT Iteration and Convergence Parameters dialog box
11.
Select “1..On” from the Auto Increment drop down menu in the Analysis Control section. Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Surface to Surface Contact Results The Advanced Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
from the View Toolbar
31-12 4.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 75, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “60031..Solid Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the Post Toolbar and select Actual Deformation from the drop down list (Must have a check mark next to it in the menu)
If the “Undeformed model” is already NOT visible, skip this portion of the step:
Click the Post Options icon from the Post Toolbar again and select Undeformed from the drop down list (Must NOT have a check mark next to it in the menu)
Post-Processing the Surface to Surface Contact Results
The deformation and stress results should look like this:
What
View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
31-13
31-14 4.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.01” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 75, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The Contact between the Clip and the Base can be viewed in this mode as the objects come into contact.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the Surface to Surface Contact - Advanced Nonlinear (SOL 601) example. It is recommended to save the model file.
32.
Analysis of a Simple Assembly
In this example, you will create a model of a simple assembly using contact conditions automatically generated by FEMAP, then solve the model two times using NX Nastran, once using “Glued Contact” and once using “Linear Contact”. Also, this example makes extensive use of the Model Info tree and Select Toolbar.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the assembly
•
creating connections between different parts of the assembly
•
meshing the model
•
applying constraints and loads
•
analyzing the model using the NX Nastran solver (Glued and Linear)
•
post-processing the results
Importing the Geometry What Import a FEMAP geometry file containing the geometry of the assembly.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the FEMAP Examples directory. Import the Assembly.x_t file.
32-2 Step
UI
Analysis of a Simple Assembly
Command/Display
2.
Solid Model Read Options dialog box: OK
3.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 4.
View Rotate dialog box: Trimetric OK
Creating Connections You will be creating connections between the different parts of the assembly. In this example, the connections will be contact conditions which NX Nastran will use during the solving process to have the parts interact with one another. In general, there are three separate entities needed to create a connection in FEMAP: Connection Property - A specific property used to set-up contact conditions for a specific solver or analysis type. We will be using the “NX Linear” tab and the Defaults button for this example. Connection Regions - Regions designated in the model which can be placed into contact with any number of other regions. Regions can be created using different types of entities such as surfaces, elements, and properties. In this example, you will create contact between the different solid parts using the surfaces of those solids. Connectors - Connectors create “contact pairs” between Connection Regions (using a Master/Slave relationship) and the contact between those regions is governed by the values set in the specified Connection Property for each Connector. Each of these entities can be created individually using the Connect menu, but FEMAP offers a few methods for creating them in a more streamlined manner. One method is to use the Connect, Surfaces command which simply allows you to choose a surface (or set of surfaces) to “connect” to another surface (or set of surfaces). The surfaces in each set will be used to create the Connection Regions, a Connection Property can be chosen (or created from inside this command), and then a single Connector will be created between the selected surfaces.
Automatic Connection Creation
32-3
In this example, we will be using the Connect, Automatic command. This creates connections automatically based on the proximity of geometric entities selected in your model using a number of parameters. These parameters include specific values for Tolerance (distance between bodies) and Angle Tolerance, as well as choice of a “Detection Strategy” (Minimal to Aggressive) and options for the way multiple Connection Regions will be combined on the same solid.
Automatic Connection Creation What Create connections automatically between the parts of the assembly.
How Step
UI
Command/Display
1.
Connect, Automatic... Menu
2.
Entity Selection dialog box: Select All OK The Auto Detection Options for Connections dialog box, should have the following values selected:
If it does not, make sure all of the above options are chosen. Then... 3.
Click OK In the Entity Selection dialog box: Click Cancel
32-4 Step
UI
Analysis of a Simple Assembly
Command/Display Tip: Creating connections automatically can also be accomplished by using the “context sensitive menu” for the Geometry branch in the Model Info tree. Simply highlight the top-level Geometry branch in the tree (or individual solids), then click the right mouse button and choose Automatic Connection from the menu. This will bring up the Connect, Automatic command
You will notice the there are new Connection Regions which are visible where the parts come together.
You can take a closer look at each Connection Property, Connection Region, and Connector which were created using the Connections branch of the Model Info tree.
Examining Created Connections Using a few “context sensitive menu” commands from the Connections branch of the Model Info tree, you can graphically see the different Connection Regions and Connectors which were created by the Connect, Automatic command. If it is not open, you will need to have the Model Info tree open for this step.
What Use the Model Info tree to examine the connections in the model.
Examining Created Connections
32-5
How Step
UI
Command/Display
1. Menu
If the Model Info tree is NOT already open, you can bring it up using the Tools, Model Info command to make it visible.
Tip: If you are not familiar with the Model Info tree or the other “dockable panes” in FEMAP, you can find more information about them using the Help, Dockable Panes... menu. The “dockable panes” contain a tremendous amount of features. It is highly recommended to take a look at the documentation for these very helpful tools. 2.
In the Model Info tree, expand the Connections branch (click on the “+” sign to the right of the title) to see the different Connection entities
You will notice that Connection Properties, Connection Regions, and Connectors are all available in the Model Info tree. 3.
Expand the Connectors branch to view the Connectors in the model
You will notice that two Connectors were created in the model by the automatic contact detection. They are listed in the following format: #(number of Connector)..Region “#-#” (“Master” Connection Region - “Slave” Connection Region). Highlight “1..Region 1-2” by clicking on it.
32-6 Step 4
UI
Analysis of a Simple Assembly
Command/Display Click the right mouse button on the highlighted Connector. When the “context sensitive” menu appears, choose the Show Master command.
You will notice that the “Master” Connection Region of Connector “1” has been highlighted in Yellow and labeled and the rest of the parts have been made transparent in the model. If your display does not look like the one below, please see the “notice” below this cell.
The model will remain in this display state until Windows, Regenerate (Ctrl+G) has been used or a command which includes a “Regenerate” (such as an entity creation command) has been performed. Notice: The Show Master and Show Slave commands follow the current settings in the Windows, Show Entities command. By default, nothing is set in FEMAP and you will get the figure above when using the Show Master and Show Slave commands. If you have changed any of the settings in the Windows, Show Entities command itself or the Show When Selected commands in the Model Info tree or Data Table, then the Show Master and Show Slave commands will use those settings.
Examining Created Connections
Step 5
UI
32-7
Command/Display Click the right mouse button on the highlighted Connector. When the “context sensitive” menu appears, choose the Show Slave command.
Tip: Although it does not matter for this model, in some cases you may want to “swap” the “Master” and “Slave” Connection Regions. This can be accomplished by using the Reverse command in the Connectors “context sensitive” menu
Tip: It is also possible to “Enable” and “Disable” Connectors in FEMAP. This allows you to choose which Connectors will be exported out of FEMAP for analysis. With this capability, you do not have to delete and recreate Connectors when determining which parts should be coming into contact in certain scenarios.
32-8
Analysis of a Simple Assembly
Applying Loads and Constraints For loads, create a load on front surface of the “Plunger”, normal to the surface. Next, create a “pinned” boundary condition using the surfaces of the rear holes of the “Baselink”.
What Create a load set, then apply a force “normal” to the front surface of the “Plunger”.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Create or Activate Load Set dialog box: Title: Normal Force
3.
Click OK
For the selection of the surface to load, use the Select Toolbar (Shown Undocked)
If the Select Toolbar is not visible, you can make it visible using the Tools, Toolbars, Select command or by right-mouse clicking in any area where a toolbar can be “docked” and choosing Select from menu. For more information on where a toolbar can be “docked”, please use the Help, Toolbars, Using the Toolbars command to view the documentation. All of the icons on the Select Toolbar are actually menus which allow you to modify the way the Select Toolbar will be used. For more information on the Select Toolbar, please view the documentation specifically created for it using the Help, Toolbars, Select command. 4. Menu
Using the Selector Entity menu on the Select Toolbar (first icon), select Surface. You will notice that the icon on the Select Toolbar has changed to the Select Surface icon.
This will make Surfaces “Active” in the Selector. Having an “Active” entity in the Selector allows you to choose Surfaces in the model before selecting any commands. In this case you will only be selecting one surface at a time, but there are options for selecting multiple surfaces, then choosing commands. This also will give you access to the “context sensitive menu” for the “Active” Entity Type in the graphics window.
Applying Loads and Constraints
Step 5.
UI
32-9
Command/Display With Surface “Active” in the Select Toolbar: Pick the front round surface of the “Plunger” (surface 36). If you turn on the Entity Info dockable pane, you will be able to see which surfaces you are choosing as you pick them. Use the Tools, Entity Info command to open up this pane.
Note: The surface will NOT change color (This has been done for this example to show which surface to select), but the small “Selected Marker” (circle in above figure) will appear in FEMAP to let you know the surface has been selected. 6.
Click the right mouse button on the highlighted Surface or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Load command. This will bring up the Create Loads on Surfaces dialog box. Tip: When the Select Toolbar has an “Active” entity type, a right mouse click in the graphics window will always bring up the “context sensitive menu” for the “Active” Entity Type. Because of this, you will not be able to use the “normal right-mouse menu” simply by clicking the right-mouse button. Instead you have to hold down the Alt key, then click the rightmouse button to get to the “normal right-mouse menu”. When there is no longer an “Active” Entity Type in the Select Toolbar, holding down Alt is not required. Tip: You can also use icons from various toolbars to perform commands on the entities in the currently in the Selector. In this case, you could have used the Create Load on Surface icon on the Loads Toolbar. Create Load on Surface icon
7.
In the Create Loads on Surfaces dialog box: Choose Force from the list of loads, if it is not already chosen.
8.
In the Direction section of the Create Loads on Surfaces dialog box: Select Normal to Surface
32-10 Step
UI
Analysis of a Simple Assembly
Command/Display
9.
In the Load section of the Create Loads on Surfaces dialog box, enter the following value: Magnitude: 100
10.
Click OK
What Create a constraint set, then create “pinned” constraints on the surfaces of the rear holes of the “Baselink”.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Title: Pinned
3.
Click OK
4. Menu
Surfaces should still be the “Active” entity type in the Select Toolbar. If there is no “Active” entity, use the Selector Entity menu on the Select Toolbar (first icon) to select Surface.
Tip: The Select Toolbar remembers the last entity type which was “Active” and a shortcut to make that entity “Active” again is to simply click the Selector Entity icon. Once you are done using the Select Toolbar, click the icon again and it will toggle back to the “no active entity” icon. This is very helpful when going back and forth between using the select toolbar and using FEMAP in the more “traditional” manner (i.e. selecting commands, then entities, then performing the actual command).
Applying Loads and Constraints
Step
UI
32-11
Command/Display
5.
Using the Selector Mode menu (second icon on the Select Toolbar), choose Select Multiple. Menu
This will allow you to choose multiple entities of the current “Active” entity types and create a “Selection List”. You can actually change the “Active” entity and place multiple entities of different types into the same Selection List. Tip: The Selection List can be viewed at the bottom of the Model Info tree. The entity types currently in the Selection List will be listed and the number of each entity type currently in the list will be shown in parenthesis after the entity type name
If you right-click any entity type in the Selection List, you will notice the same “context sensitive menu” will appear for each entity type, as when the entity type is active in the Select Toolbar. This can be an excellent way to get to commonly used commands when you are performing operations on different entity types.
32-12 Step 6.
UI
Analysis of a Simple Assembly
Command/Display With Surface “Active” in the Select Toolbar: Pick the 4 surfaces of the rear holes of the “Baselink” (surfaces 1, 2, 31, and 32).
Note: The surfaces will NOT change color (This has been done for this example to show which surfaces to select), but the small “Selected Markers” (circles in above figure) will appear in FEMAP to let you know the surfaces have been selected. 7.
Click the right mouse button on any of the highlighted Surfaces or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Constraint command. This will bring up the Create Constraints on Surfaces dialog box.
8.
Create Constraints on Geometry dialog box: Pinned - No Translation
9.
Click OK
Meshing the Model
32-13
Meshing the Model You will be using the Model Info tree to select the solids to mesh and then a command from the Solid “context sensitive menu” to actually mesh the assembly. This will reduce the number of commands needed to create the mesh by prompting you to create a material and automatically creating the correct type of property required for solid tetrahedral meshing.
What Mesh the solids using the Model Info tree.
How Step 1.
UI
Command/Display In the Model Info tree, expand the Geometry branch (click on the “+” sign to the right of the title) to see the different Geometry entities (only Solids are in the tree)
Highlight all of solids by selecting the first solid in the list (1..Baselink), then holding the Shift key down and selecting the last solid in the list (3..Pin). 2.
Click the right mouse button on the highlighted Solids. When the “context sensitive menu” appears, choose the Tet mesh command.
32-14 Step
UI
Analysis of a Simple Assembly
Command/Display
3.
FEMAP will prompt you to make a material to be used for all of the selected Solids Define Material - ISOTROPIC dialog box: Click Load
4.
Select from Library dialog box: AISI 4340 Steel (select)
5.
Click OK, then... In the Define Material - ISOTROPIC dialog box: Click OK Tip: You will notice that the model has been sized for meshing. If you want to change the mesh size to anything but the default value, you can do this by clicking the Update Mesh Sizing button in the Automesh Solids dialog box. For this example, the default mesh size is fine.
6.
In the Automesh Solids dialog box: OK The model is now meshed and now is a good time to turn off the Geometry and some other entities in the graphics window.
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
8.
In View Quick Options dialog box: Click All Entities Off button, then...
9.
CHECK Element box located in the Mesh section, then
10.
Click Done
Notice: The Loads and Constraints are still applied to the model, they are just no longer visible. If you want to turn then on to verify they are there, simply use Ctrl+Q again and press the Load/Constraint On button and then Done. For this example, we are turning them off now for Post-Processing after the model has been solved.
Analyzing the “Glued Contact” Model
Step
UI
32-15
Command/Display
THE MODEL IS NOW READY TO BE ANALYZED!
Analyzing the “Glued Contact” Model The FEMAP analysis manager stores the options for creating an input file for a solver (an analysis set). It can launch the NX NASTRAN solver or another solver that has been set up to run on the same PC. The analysis manager, together with VisQ, can also set up and run analyses with solvers on other PCs. The analysis sets are stored with the FEMAP model file, and can also be stored in a FEMAP library that can be accessed from different model files.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Tip: You can also create a new Analysis Set using the Manage command on the “context sensitive menu” located on the Analyses branch in the Model Info tree (simply click to highlight the top level of the Analyses branch or any existing Analysis Set, then right mouse click to see the context sensitive menu). 2.
Analysis Set Manager dialog box: New
3.
Analysis Set dialog box: Title: Glued Contact
4.
Analysis Program: 36..NX Nastran Analysis Type: 1..Static
32-16 Step
UI
Analysis of a Simple Assembly
Command/Display
5.
Click OK
Notice: The analysis set manager displays all analysis sets defined in the model, and the sections that make up the input file for the solver. Clicking on a plus sign will expand the tree and display individual options that can be edited by double-clicking on an option. For this analysis, you’ll use the default values for these options. 6.
Analyze
Notice: The Analysis Monitor window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results of “Glued Contact” Analysis For this example, you will display the Deformed Shape and Contour Plot of the Solid von Mises Stress.
What Display the deformed model and the Solid von Mises Stress.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Set: 1..NX Nastran Case 1 In Output Vectors: Deformation: 1..Total Translation Contour: 60031..Solid Von Mises Stress
5.
OK (all dialog boxes)
Modifying the Connection Property
Step
UI
32-17
Command/Display
You can perform some other Post-processing commands on this model, then save the model. For some interesting Post-processing options for Solid Elements, such as Dynamic Cutting Plane and Dynamic Isosurface, see Example 7: Using postProcessing. At this point, we will now modify the Connection Property and add a Constraint to run the Model again using “Linear Contact” instead of “Glued Contact”. To do this, you will again access a command via a “context sensitive menu” from the Model Info tree.
Modifying the Connection Property What Modify the Connection Property using the Model Info tree.
How Step 1.
UI
Command/Display In the Model Info tree, expand the Connections branch (click on the “+” sign to the right of the title) to see the different Connection entities
32-18 2.
Analysis of a Simple Assembly
Expand the Properties branch to view the Connection Properties in the model
You will notice there is only one Connection Property in the model. You are going to modify this property and then run the analysis again. 3.
Click the right mouse button on the highlighted Connection Property. When the “context sensitive” menu appears, choose the Edit command.
4.
In the Define Connection Property dialog box: Change the Connect Type from “1..Glued” to “0..Contact”
Notice: The NX Linear tab is currently active. When you change the Connect Type from “1..Glued” to “0..Contact” certain fields are made “inactive” (greyed out) and other fields become available. In this case, we will just use the default values for “Linear Contact” in this exam 5.
Click the Defaults button at the bottom of the Define Connection Property dialog box
6.
In the Contact Pair (BCSET) section, enter the following value: Friction: 0.2
7.
Click OK
Now you will return the model to a view where another constraint can be added easily.
Modifying the Connection Property
What Display only the Geometry, Loads and Constraints in an undeformed, uncontoured plot.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: None - Model Only Contour Style: None - Model Only
3.
4.
Click OK
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
5.
In View Quick Options dialog box: Click Analysis Entities Off button, then... Click Geometry On button, then... Click Load/Constraint On button, then... Click Done
32-19
32-20
Analysis of a Simple Assembly
Applying additional Constraints for stability You may need to place a few more constraints on the model to keep the “Pin” from sliding out of the holes in the “Baselink” and the “Plunger”.
What Create some “sliding along surface” constraints set on the two ends of the “Pin”
How Step
UI
Command/Display
1. Menu
Surfaces might still be the “Active” entity type in the Select Toolbar depending on what other post-processing you did on the Glued Contact model. If there is no “Active” entity, use the Selector Entity menu on the Select Toolbar (first icon) to select Surface. Tip: The Select Toolbar remembers the last entity type which was “Active” and a shortcut to make that entity “Active” again is to simply click the Selector Entity icon. Once you are done using the Select Toolbar, click the icon again and it will toggle back to the “no active entity” icon.
2.
Clear the Selector using the Selector Clear icon (4th icon from the left on Select Toolbar).
This will clear the Selection List. Tip: Along with clearing the entire Selection List, you can instead use the Clear Active Entity command on the Clear Selector Menu.
This will only remove the entities from the Selection List which are the same entity type as “Active” entity type in the Select Toolbar. This is very helpful if you are creating a large Selection List with many different entity types. 3.
With Surface “Active” in the Select Toolbar: Pick the surfaces at each end of the “Pin” (surfaces 41 and 42). If you turn on the Entity Info dockable pane, you will be able to see which surfaces you are choosing as you pick them. Use the Tools, Entity Info command to open up this pane. Tip: You may need to rotate the model to pick both of these surfaces. When the Select Toolbar has an “Active” entity type, you can rotate the model using by holding down the middle mouse button or wheel and then moving the mouse around.
Analyzing the “Linear Contact” Model
Step
UI
32-21
Command/Display
4.
Click the right mouse button on any of the highlighted Surfaces or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Constraint command. This will bring up the Create Constraints on Surfaces dialog box.
5.
Create Constraints on Geometry dialog box: Select Surface, then... Select Sliding along Surface (Symmetry)
6.
Click OK
Note: The surfaces will NOT change color (This has been done for this example to show which surfaces to select), but the small “Selected Markers” (circles in above figure) will appear in FEMAP to let you know the surfaces have been selected. THE MODEL IS NOW READY TO BE ANALYZED!
Analyzing the “Linear Contact” Model What Analyzing the model via a “context sensitive menu” from the tree.
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: Click Analyze
32-22 Step
UI
Analysis of a Simple Assembly
Command/Display Tip: You can also get to an existing Analysis Set using the Manage command on the “context sensitive menu” located on the Analyses branch in the Model Info tree (simply click to highlight the top level of the Analyses branch or any existing Analysis Set, then right mouse click to see the context sensitive menu). Also, if you already have an Analysis Set created, you can simply use the Analyze command on the Analyses branch “context sensitive menu”. If you only have one analysis set, FEMAP will run it from the top-level Analyses branch. If you have multiple Analysis Sets, select an individual Analysis Set and then use the context sensitive menu to Analyze that set. Notice: The Analysis Monitor window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results of “Linear Contact” Analysis For this example, you will again display the Deformed Shape and Contour Plot of the Solid von Mises Stress.
What Display the deformed model and the Solid von Mises Stress.
How Step
UI
Command/Display
1.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
2.
In View Quick Options dialog box: Click All Entities Off button, then...
3.
CHECK Element box located in the Mesh section, then
4.
Click Done
5.
View, Select Menu
6.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
Post-processing the Results of “Linear Contact” Analysis
Step
UI
32-23
Command/Display
7.
Deformed and Contour Data
8.
Select PostProcessing Data dialog box: Output Set: 2..NX Nastran Case 1 In Output Vectors: Deformation: 1..Total Translation Contour: 60031..Solid Von Mises Stress Notice: The displacements and stresses are quite a bit higher for the “Linear Contact”. This is because the model was allowed to move much more compared to when the model was “Glued” together.
9.
OK (all dialog boxes)
10.
Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the drop down list
from the Post Toolbar and select Actual Deformation
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting Postprocessing as the category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Post Options menu on the Post Toolbar for this task 11.
Turn off the “Filled Edges” in the model using the View Style Menu on the View Toolbar.
Select Filled Edges from the View Style and the lines representing the elements will no longer be visible. This cleans up the view somewhat for creating pictures.
32-24 Step
UI
Analysis of a Simple Assembly
Command/Display
Again, you can perform some other Post-processing commands on this model, then save the model. For some interesting Post-processing options for Solid Elements, such as Dynamic Cutting Plane and Dynamic Isosurface, see Example 7: Using post-Processing. This is the end of the example. You don’t need to save the model file.
Index A advanced post options 7-4 analysis buckling 3-1, 32-1 analysis manager 3-11, 11-16, 12-10, 13-14, 14-12, 32-15 animation AVI 7-16 copy to other applications 7-14 speed 7-15 AutoCad file 12-1 AVI file 7-16 axisymmetric model 12-1
B beam 11-1 cross section 11-4 property 11-2 beam diagram 11-20 boundary conditions applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 boundary surface 3-3, 4-2, 8-4, 12-5, 32-13 break 4-5 buckling 3-1, 32-1
C cache pages 2-11 cleanup 9-5, 9-7 coincident nodes 3-7, 11-11, 32-15 constraint fixed 4-16, 8-10, 32-8 nodal 11-12 symmetry 4-16, 8-10, 11-12, 32-8 constraints applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 nodal 3-8, 12-7, 13-12, 32-15 on curves 14-11 symmetric 13-12 contour data 3-12, 7-1, 7-2, 12-11, 32-16 contour options 7-4 criteria data 11-17 cross section beam 11-4 display 11-7 Ctrl-Z 9-3 curve 4-4, 4-10 list 9-6 cutting plane 7-4
D deformed data 3-12, 7-1, 7-2, 11-17, 12-11, 32-16 degenerate surface 8-1
delete 13-3, 13-6, 14-4, 14-7 DXF file 12-1 Dynamic Analysis Direct Transient 15-1 Modal Frequency 16-1, 17-1 Random Response 18-1 Response Spectrum 19-1 Dynamic Analysis Parameters Direct Transient 15-7, 19-8 Modal Frequency 16-9, 17-6, 18-7 dynamic cutting plane 7-6 dynamic isosurfaces 7-6
E element beam 11-1 create 10-5 display 6-4, 11-7 fill 6-5 properties 6-4 properties and materials 3-2, 4-18, 11-2, 12-3, 32-13 rod 11-9 shrink 6-5 errors starting 2-8 explode 9-5 extrude 4-2, 4-7
F feature suppress 8-2, 8-6 file DXF 12-1 STP 14-1 X_T 8-2, 9-1, 13-1 fill 6-5 free body display 13-15, 13-17, 14-12 free edge 3-6, 10-2, 32-15, 1-1 functions 15-3
G geometry import 3-1, 4-1, 8-2, 9-1, 10-1, 11-1, 12-1, 13-1, 14-1, 32-1 meshing 3-3, 4-18, 32-13 repair 9-1 sliver 9-1 geometry mesh options 11-9 graphics copy to other applications 7-12 graphics boards 2-1 group 5-1 create 5-1, 5-3, 5-6, 10-3, 13-15 display 5-3
I-2
Index
model data 5-7, 10-3 plot 7-10 report 5-4
H hardware requirements 2-1 hidden line 6-2 hide layer 5-9
I import AutoCad DXF file 12-1 model file 5-1 neutral file 3-1, 4-1, 10-1, 11-1, 32-1 Parasolid X_T file 8-2, 9-1, 13-1 STP file 14-1 Installation PC Network 2-5 PC Stand Alone 2-1 isosurface 7-4
L layer 5-1, 5-9 view 5-9, 11-5 license file 2-5 line 4-12 loads applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 elemental 12-8 nodal 3-10, 11-15 on curve 13-10 on surfaces 14-10
M manual conventions 1-3 mass properties 9-2 material defining 3-2, 4-18, 11-2, 12-3, 32-13 merge nodes 11-11 mesh 4-18 curve 11-6, 11-9 repair 10-1 solid 8-7, 9-3, 9-9, 10-6 surface 3-3, 3-5, 12-5, 13-8, 14-9, 32-13 mesh attributes 13-8, 14-8 mesh size 3-4, 12-2, 13-8, 14-9, 32-15 midsurface 13-1, 14-1 create 13-4, 14-2 model import 5-1 open 6-1 model data 5-7, 6-3 model file 5-1, 6-1 model style 6-2
N network licensing 2-5 neutral file 3-1, 4-1, 10-1, 11-1, 32-1 nodes coincident 3-7, 11-11, 32-15 Nonlinear Gap Contact 26-1 Large Deformation 27-1 Plastic Deformation 25-1 Slide Line Contact 28-1 Snap Fit Contact 29-1
O open model file 6-1 output set 7-9 overview FEMAP 1-1
P Parasolid file 8-2, 9-1, 13-1 part creating 4-2 pattern 4-8 plots 7-1, 7-2 post-processing 3-12, 7-1, 11-17, 12-11, 13-15, 14-12, 32-16 pressure 12-8, 14-10 properties groups 5-6 property beam 11-2 defining 3-2, 4-18, 11-2, 12-3, 32-13
Q quick options 11-11
R RAM Management 2-11 render 6-2 report create 5-4 results 3-12, 11-17, 12-11, 13-15, 14-12, 32-16 reverse normal direction 11-8 rotate 11-6
S security device 2-2, 2-10 upgrading 2-4 show 5-5 layer 5-9 shrink 6-5 slice 8-3, 13-2 sliver geometry 9-1 software requirements 2-1 solid model
Index
analyzing 4-1 solids from elements 10-6 solving 3-11, 11-16, 12-10, 13-14, 14-12, 32-15 Starting FEMAP 2-8 Step file 14-1 stitch 9-2, 9-8, 13-7 surface degenerate 8-1 prepare for meshing 8-1 stitch 9-2 symmetry constraint 4-16, 8-10, 11-12, 13-12, 32-8
U
T
workplane 4-12
The 1-3 Thermal Analysis Enclosure Radiation 24-1 Free Convection 22-1 Steady State Heat Transfer 21-1 Temperature Dependency 23-1 Thermal Stress 20-1 trim with curve 14-5
undo 9-3 update elements 11-8
V view options 6-3 view select 6-1
W X X_T file 8-2, 9-1, 13-1 XY plot 7-7
Z zoom 11-8
I-3
I-4
Index
Version 9.3
Proprietary and Restricted Rights Notice © 2007 UGS Corp. All Rights Reserved. This software and related documentation are proprietary to UGS Corp. All trademarks belong to their respective holders.
UGS Web:
http://www.femap.com
Customer Support Phone: Web:
(714) 952-5444, (800) 955-0000 (In US & Canada) http://support.ugs.com
Conventions This manual uses different fonts to highlight command names or input that you must type.
a:setup
Shows text that you should type.
OK, Cancel
Shows a command name or text that you will see in a dialog box.
Throughout this manual, you will see references to Windows. Windows refers to Microsoft® Windows 2000, Windows Me, or Windows XP. You will need one of these operating environments to run FEMAP for the PC. This manual assumes that you are familiar with the general use of the operating environment. If you are not, you can refer to the Windows User’s Guide for additional assistance. Similarly, throughout the manual all references to FEMAP, refer to the latest version of our software. Special note for customers using Windows Vista: FEMAP 9.3 is being released close to the same time as the initial release of Windows Vista. Currently, Windows Vista is an “unsupported” platform. Although we have tested FEMAP on Windows Vista with much success, there are issues with many graphics cards and drivers not being available for Vista at this time, which may cause issues in FEMAP.
FEMAP Examples Proprietary and Restricted Rights Notice 1. Introduction Introduction to FEMAP . . . Using the FEMAP Examples Guide The FEMAP Documentation Set .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. 1-1 . 1-3 . 1-5
Hardware/Software Requirements . . . Installation - Stand Alone . . . . Network Installation - PC . . . . Improving Performance (RAM Management) Memory Setting Guidelines . . . . Licensing Conversion Methods . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. 2-1 . 2-1 . 2-5 2-11 2-12 2-12
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 3-1 . 3-2 . 3-8 3-12
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 5-1 . 5-1 . 5-9 5-11
2. Installing FEMAP
3. Analyzing Buckling for a Bracket Importing the Geometry . . Meshing the Model . . . Applying Constraints and Loads Post-processing the Results .
. . . .
. . . .
. . . .
. . . .
4. Creating and Meshing a Solid Model Importing the Geometry . . Creating the Solid Part . . Creating the Slot . . . Creating the Bolt Holes . . Creating the Guide Boss . . Applying Constraints and Loads Meshing the Model . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
5. Working with Groups and Layers Differences Between Groups and Layers Using Groups . . . . . . Using Layers . . . . . . Using a Contour Group for Post-processing
. . . .
. . . .
6. Working with View Select and View Options Using View Select . Using View Options
. .
. .
. .
. .
4-1 4-2 4-4 4-8 4-10 4-16 4-18
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. 6-1 . 6-3
Post Processing Overview . . . . Generating Deformation and Contour Results Generating XY Plots . . . . . Using Results Displays in Other Applications
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. 7-1 . 7-1 . 7-7 7-12
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
8-1 8-2 8-4 8-6 8-7 8-9
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
9-1 9-2 9-3 9-4
7. Using Post-Processing
8. Preparing Geometry for Meshing Understanding the Problem . Preparing the Geometry . . Creating New Boundary Surfaces Suppressing Features . . Meshing the Model . . . Applying Loads and Constraints
. . . . . .
. . . . . .
. . . . . .
. . . . . .
9. Repairing Sliver Geometry for Meshing Importing the Geometry . . Stitching the Surfaces . . Meshing the Model . . . Repairing Problem Geometry .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
TOC-2 Meshing the New Solid
.
10. Repairing a Mesh Importing the Mesh . Examining Free Edges Repairing Mesh Problems Meshing the Model .
. . . .
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
9-8
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
10-1 10-2 10-3 10-6
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
11-1 11-2 11-5 11-12 11-16 11-17
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
12-1 12-2 12-7 12-10 12-11
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
13-1 13-2 13-4 13-8 13-10 13-14 13-15
11. Analyzing a Beam Model Importing the Geometry . . Defining the Material and Property Meshing the Model . . . Applying Constraints and Loads. Analyzing the Model . . . Post-Processing the Results .
. . . . . .
12. Analyzing an Axisymmetric Model Importing the Geometry . . Meshing the Model . . . Applying Constraints and Loads. Analyzing the Model . . . Post-processing the Results .
. . . . .
. . . . .
. . . . .
. . . . .
13. Analyzing a Midsurface Model of a Welded Pipe Importing the Geometry . . Slicing the Model . . . Creating the Midsurface Model . Meshing the Model . . . Applying Loads and Constraints. Analyzing the Model . . . Post-processing the Results .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
14. Analyzing a Midsurface Model of an Electrical Box Importing the Geometry . . Creating the Midsurface Model . Meshing the Model . . . Applying Loads and Constraints. Analyzing the Model . . . Post-processing the Results .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
15. Direct Transient Analysis – Hinge Model Importing the Model . . . . . Creating the Transient Load . . . Defining the Transient Analysis Parameters Setting up the Analysis Set Manager . . Post-Processing the Results . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
14-1 14-2 14-8 14-10 14-12 14-12
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
15-2 15-6 15-7 15-10 15-12
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
16-1 16-3 16-5 16-12 16-14 17-2 17-5 17-8 17-10 17-13 17-14 17-16 17-18 17-19
16. Modal Frequency Analysis of the Hinge Model Importing the Neutral File . . . . . . Running the Normal Modes Analysis. . . . Creating Unit Load for Frequency Response Loading Running the Modal Frequency Response Analysis . Post-Processing the Results . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
17. Frequency Response of Tower with Seismic Excitation Importing the Model . . . . . Creating Function for Seismic Loading . Creating the Base Node and Rigid Connection Large Mass Method . . . . . Running the Seismic Analysis . . . Post-Processing the Results . . . Direct Method . . . . . . Running the Seismic Analysis . . . Post-Processing the Results . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
18. Random Response of the Hinge Model Opening an Existing FEMAP Model . . . . . Defining the Power Spectral Density Function . . . Creating Enforced Motion Loading - Large Mass Method
. . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . . . . . . . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. 18-1 . 18-3 . 18-7
TOC-3 Creating Enforced Motion Loading - Direct Method Setting the Random Response Parameters . . Creating a Group for Output Request needs . . Running the Random Response Analysis . . Post-Processing the Random Response Analysis .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
19. Generation of Response Spectra - Single Degree of Freedom model Creating the Model . . . . . . . . Creating the Dynamic Loading Function . . . Creating the Load . . . . . . . . Setting the Response Spectrum Generation Parameters . Setting up the Analysis Set Manager . . . . Post-processing - Response Spectrum Generation . .
20. Thermal Stress Analysis -
. . . . . .
. . . . . .
. . . . . .
Mounting Plate
Importing the Model . . . . . . . Creating the Thermal Boundary Conditions . . . Running the Steady-State Thermal Analysis . . . Post-Processing the Thermal Results . . . . Creating Nodal Temperatures from the Thermal Results Running the Thermal Stress Analysis . . . . Post-Processing the Thermal Results . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . .
. . . .
. . . .
. . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
19-1 19-3 19-5 19-8 19-10 19-12
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
20-2 20-3 20-7 20-8 20-9 20-12 20-13
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
21-1 21-4 21-8 21-9
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
22-1 22-2 22-4 22-5
. . . . . . . .
23. Temperature - Dependent effects - Circuit Board Opening an Existing FEMAP Model . . . . . Creating a Temperature Dependent Material Property . . Creating a Temperature Dependent Convection Coefficient (h) Running the Steady-State Thermal Analysis . . . . Post-Processing the Thermal Results . . . . .
24. Enclosure Radiation
Opening a FEMAP Model . . . . . Creating Materials and Properties . . . . Reversing the Element Normals . . . . Creating Radiation Emissivity and Heat Flux Loads Running the Steady-State Thermal Analysis . . Post-Processing the Thermal Results . . .
. . . . . .
. . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
23-1 23-2 23-5 23-8 23-9
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
24-1 24-2 24-6 24-9 24-14 24-15
25. Plastic Deformation of Rod - Nonlinear Material Creating the Nonlinear Material . . . . Creating the Property and Mesh . . . . Creating Loads and Constraints . . . . Running the Nonlinear Static Analysis with two cases Post-Processing the Results . . . . .
26. Gap Contact - Cantilever Beam Creating the Geometry . . . . Creating the Materials and Properties . Creating the Gap property and element . Creating the loads and constraints . . Creating Settings for Nonlinear analysis Running the Nonlinear Static Analysis . Post-Processing the Gap Contact Results
. . . . . . .
. . . . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
25-1 25-5 25-7 25-11 25-14
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
26-1 26-2 26-6 26-9 26-11 26-13 26-14
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
. .
27-1 27-3
27. Large Deformation - Cantilever Beam Creating the Geometry . . . Creating the Materials and Properties
. .
. .
. .
18-12 18-15 18-17 18-18 18-20
. . . . . .
22. Steady - State Thermal Analysis - Free Convection Opening an Existing FEMAP Model . . . Creating the Free Convection Boundary Conditions Running the Steady-State Thermal Analysis . . Post-Processing the Thermal Results . . .
. . . . .
. . . . . .
21. Steady - State Thermal Analysis - Circuit Board Importing the Model . . . . . . . . . . Creating the Heat Generation Loads and Thermal Boundary Conditions Running the Steady-State Thermal Analysis . . . . . . Post-Processing the Thermal Results . . . . . . .
. . . . .
. .
. .
TOC-4 Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Large Deformation Results
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
27-10 27-12 27-13 27-14
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
. . . . . . .
28-2 28-3 28-4 28-8 28-13 28-14 28-15
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
. . . . . .
29-2 29-3 29-7 29-9 29-10 29-11
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
30-1 30-3 30-5 30-8
28. Slide Line Contact - Hyperelastic Seals Importing the Neutral File . . . . . Modifying the Material . . . . . Creating the Slide Line Property and Element . Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Slide Line Contact Results .
. . . . . . .
. . . . . . .
29. 3-D Contact - Plastic Clip and Base Importing the Neutral File . . . . . Creating the Contact (Slide Line) Element. . Creating the loads and constraints . . . Creating Settings for Nonlinear analysis . . Running the Nonlinear Static Analysis . . Post-Processing the Slide Line Contact Results .
. . . . . .
. . . . . .
30. Large Deformation - Advanced Nonlinear (SOL 601) Importing the Neutral File . . . . . Creating the functionally dependent loads . . Running the Nonlinear Static Analysis . . Post-Processing the Large Deformation Results
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
31. Surface to Surface Contact - Advanced Nonlinear (SOL 601) Importing the Neutral File . . . . . . Creating the Contact Conditions. . . . . Creating the loads and constraints . . . . Running the Nonlinear Static Analysis . . . Post-Processing the Surface to Surface Contact Results
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
31-2 31-3 31-6 31-9 31-11
Importing the Geometry . . . . . . . Creating Connections . . . . . . . . Applying Loads and Constraints. . . . . . Meshing the Model . . . . . . . . Analyzing the “Glued Contact” Model . . . . Post-processing the Results of “Glued Contact” Analysis . Modifying the Connection Property . . . . . Applying additional Constraints for stability . . . Analyzing the “Linear Contact” Model . . . . Post-processing the Results of “Linear Contact” Analysis.
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
. . . . . . . . . .
32-1 32-2 32-8 32-13 32-15 32-16 32-17 32-20 32-21 32-22
32. Analysis of a Simple Assembly
Index
1.
Introduction
This section introduces FEMAP and explains how to use the FEMAP Examples guide.
Introduction to FEMAP FEMAP is finite element modeling and post-processing software that allows you to perform engineering analyses both quickly and confidently. FEMAP provides the capability to develop sophisticated analyses of stress, temperature, and dynamic performance directly on the desktop. With easy access to CAD and office automation tools, productivity is dramatically improved compared to traditional approaches. FEMAP automatically provides the integration that is necessary to link all aspects of your analysis. FEMAP can be used to create geometry, or you can import CAD geometry. FEMAP provides powerful tools for meshing geometry, as well as applying loads and boundary conditions. You may then use FEMAP to export an input file to over 20 finite element codes. FEMAP can also read the results from the solver program. Once results are obtained in FEMAP, a wide variety of tools are available for visualizing and reporting on your results. With FEMAP you can: •
Import or Create Geometry
•
Build a Finite Element Model
•
Check Your Model
•
Analyze Your Model
•
Post-process Results
•
Document Results
Import or Create Geometry FEMAP can directly import geometry from your CAD or design system. In fact, FEMAP can directly import a solid model from any ACIS-based or Parasolid-based modeling package. If your modeling package does not use either of these packages, you can use the FEMAP IGES or STEP reader. If you are using I-DEAS, you can bring a single part into FEMAP by exporting a Viewer XML (IDI) file from I-DEAS. These files can be read and then stitched together to form a solid. This typically requires using one command. If you do not have CAD geometry, you can create geometry directly in FEMAP using powerful wireframe and solid modeling tools. Solid modeling directly in FEMAP uses the robust Parasolid modeling engine. You can build or modify solid models using the Parasolid engine, and then export the geometry out of FEMAP. This is very convenient if you need to export geometry to CAD packages that are Parasolid-based.
Build a Finite Element Model Regardless of the origin of your geometry, you can use FEMAP to create a complete finite element model. Meshes can be created by many methods ranging from manual creation, to mapped meshing between keypoints, to fully automatic meshing of curves, surfaces and solids. FEMAP can even work with your existing analysis models. You can import and manipulate these models using the interfaces to any of the supported analysis programs. Appropriate materials and section properties can be created or assigned from FEMAP libraries. Many types of constraint and loading conditions can be applied to represent the design environment. You can apply loads/constraints directly on finite element entities (nodes and elements), or you can apply them to geometry. FEMAP will automatically convert geometric conditions to nodal/elemental values upon translation to your solver program. You may even convert these loads before translation to convince yourself that the loading conditions are appropriate for your model.
1-2
Introduction
Check Your Model At every step of the modeling process, you receive graphical verification of your progress. You need not worry about making a mistake because FEMAP contains a multi-level undo and redo capability. FEMAP also provides extensive tools for checking your model before you analyze it to give you the confidence that you have properly modeled your part. It constantly examines input to prevent errors in the model, and provides immediate visual feedback. FEMAP also provides a comprehensive set of tools to evaluate your finite element model and identify errors that are often not obvious. For example, FEMAP can check for coincident geometry, find improper connections, estimate mass and inertia, evaluate your constraint conditions, and sum your loading conditions. Each of these methods can be used to identify and eliminate potential errors, saving you considerable time and money.
Analyze Your Model When your model is complete, FEMAP provides interface to over 20 popular programs to perform finite element analysis. You can even import a model from one analysis program and automatically convert it to the format for a different analysis program. The NX Nastran for FEMAP solver is a general finite element analysis program for structural and thermal analysis that is integrated with FEMAP.
Post-process Results After your analysis, FEMAP provides both powerful visualization tools that enable you to quickly interpret results, and numerical tools to search, report, and perform further calculations using these results. Deformation plots, contour plots, animations, and XY plots are just some of the post-processing tools available to the FEMAP user. FEMAP supports OpenGL, which provides even more capability for post-processing, including dynamic visualization of contours through solid parts. You can dynamically rotate solid contoured models with one push of your mouse button. Section cuts and isosurfaces can be viewed dynamically by simply moving your cursor.
Document Results Documentation is also a very important factor with any analysis. FEMAP obviously provides direct, high quality printing and plotting of both graphics and text. Frequently, however, graphics or text must be incorporated into a larger report or presentation. FEMAP can export both graphics and text to non-engineering programs with a simple Windows Cut command. You can easily export pictures to popular programs such as Microsoft Word, Microsoft Power Point, and Adobe Framemaker. You can export to spreadsheets, databases, word processors, desktop publishing software, and paint and illustration programs. These links enable you to create and publish a complete report or presentation, all electronically, right on your desktop. With support for AVI files, you can even include an animation directly in your Power Point Presentation or Word document. FEMAP also supports VRML and JPEG format so anyone can easily view results with standard viewers.
Using the FEMAP Examples Guide
1-3
Using the FEMAP Examples Guide The FEMAP Examples guide is designed to teach new users the basics of using FEMAP. It contains a number of examples that take you step-by-step through the processes for building and using an FEA model.
Working through the Examples As there are many different types of real analysis problems, there are different types of example problems shown here. Generally, you should start with the first example in chapter 3 and work through the examples sequentially. Some of the later examples focus on specific techniques that you may not use in your work (beam modeling, axisymmetric modeling, midsurfacing). However, we recommend that you work through all the problems because they may contain some commands or techniques that you will find useful. •
Analyzing Buckling for a Bracket
•
Creating and Meshing a Solid Model
•
Working with Groups and Layers
•
Working with View Select and View Options
•
Using Post-Processing
•
Preparing Geometry for Meshing
•
Repairing Sliver Geometry for Meshing
•
Repairing a Mesh
•
Analyzing a Beam Model
•
Analyzing an Axisymmetric Model
•
Analyzing a Midsurface Model of a Welded Pipe
•
Analyzing a Midsurface Model of an Electrical Box
•
Direct Transient Analysis – Hinge Model
•
Modal Frequency Analysis of the Hinge Model
•
Frequency Response of Tower with Seismic Excitation
•
Random Response of the Hinge Model
•
Generation of Response Spectra - Single Degree of Freedom model
•
Thermal Stress Analysis - Mounting Plate
•
Steady - State Thermal Analysis - Circuit Board
•
Steady - State Thermal Analysis - Free Convection
•
Temperature - Dependent effects - Circuit Board
•
Enclosure Radiation
•
Large Deformation - Cantilever Beam
•
Plastic Deformation of Rod - Nonlinear Material
•
Gap Contact - Cantilever Beam
•
Slide Line Contact - Hyperelastic Seals
•
3-D Contact - Plastic Clip and Base
•
Large Deformation - Advanced Nonlinear (SOL 601)
•
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
•
Analysis of a Simple Assembly
1-4
Introduction
The examples in this manual should help you learn the basic FEA modeling process, general FEMAP commands, and the FEMAP command structure. For a more complete description of the FEMAP interface and modeling procedures, see the FEMAP User Guide. For an in-depth description of all the commands in FEMAP, see FEMAP Commands.
Using the Examples In general, italicized text identifies items in the user interface. For example: File, Preferences tells you to pick the File menu, then the Preferences command. The Examples also include some graphics to help you identify user interface (UI) items. They include: UI Graphic
Meaning Pick an option from a cascading menu.
Menu
Pick an item from a pull-down menu on a dialog box.
Pick an item from a list.
Pick an icon.
Enter a value into a field on a dialog box.
Pick a button.
Pick a radio button.
Check an item on or off in a dialog box.
Pick with the left mouse button.
Pick with the right mouse button.
The FEMAP Documentation Set
1-5
Pick with middle mouse button if you have a three button mouse. Also can be the wheel of a wheel mouse.
Ctrl-A
Hold the Control key, then pick the letter key.
F5 key
Pick the function key.
The FEMAP Documentation Set FEMAP comes with a set of three printed manuals: FEMAP Examples, the FEMAP User Guide, and the FEMAP Commands reference manual. The FEMAP online help includes the contents of these manuals, as well as several additional books. The complete set includes: •
FEMAP Examples: Step-by-step examples for new users.
•
FEMAP User Guide: General information on how to use FEMAP, including an overview of the finite element modeling process. Also contains reference information for the FEMAP analysis program and geometry interfaces.
•
FEMAP Commands: Detailed information on how to use FEMAP commands.
•
FEMAP API Reference: Information on how to write your own applications that work with FEMAP.
•
What’s New: New features for this release.
When NX Nastran for FEMAP is installed, online help includes all of the above, as well as a full set of current NX Nastran documentation, to assist you during the solving portion of the analysis process.
1-6
Introduction
2.
Installing FEMAP
This section will help you install and start using the FEMAP software. This section contains information specific to getting started on a PC, which includes Windows 2000, Windows Me, and Windows XP. Special note for customers using Windows Vista: FEMAP 9.3 is being released close to the same time as the initial release of Windows Vista. Currently, Windows Vista is an “unsupported” platform. Although we have tested FEMAP on Windows Vista with much success, there are issues with many graphics cards and drivers not being available for Vista at this time, which may cause issues in FEMAP.
Hardware/Software Requirements There are no special hardware/software requirements for FEMAP beyond those imposed by Windows operating systems. There are many types of hardware that will allow you to use FEMAP. Proper choice of hardware, however, can often make the difference between frustration and productivity. Here are a few suggestions: •
Memory, RAM
•
Memory, (Hard Disk)
•
Graphics Boards
•
Browser
Memory, RAM You will need at least 32 Mbytes of RAM to run FEMAP. Furthermore, if you are going to use the solid modeling engines, 128 Mbytes of memory is required. Obviously, the more amount of RAM the better. Adding RAM can be one of the most cost effective means of increasing performance.
Memory, (Hard Disk) Required hard disk space is very difficult to estimate, but in general you will never have enough. Analysis results will be the main driver of any disk space requirement. Models are typically relatively small. A model with 1000 nodes and 1000 elements would typically be less than 1 Mbyte in size. Output from an analysis of that model, however, could be 5 Mbytes, 10 Mbytes or even larger, depending on the output you request. To estimate total disk space, you need to first estimate how many models you will have online simultaneously, the approximate size of those models, and the type of output you will request.
Graphics Boards Standard graphics adapters work very well with FEMAP. Specialized boards which contain support for OpenGL will provide increased graphical performance when dynamically rotating large, complex models. They also usually provide higher resolution and more colors, which make graphics easier to see and more realistic.
Browser To run the online help, you must have Netscape Navigator or Internet Explorer, version 4.5 or later.
Installation - Stand Alone This section describes the procedure that you should follow to install the stand alone (security device) version of FEMAP on your PC.
2-2
Installing FEMAP
Security Device Computer
FEMAP Printer
In order to run the Stand Alone (Security Device) version of FEMAP a Rainbow SuperPro Parallel Port (pictured on left) or USB Port dongle is required. In order for your PC to be able to see the dongle, a driver must first be installed. Installation of the driver requires Administrator privileges for your PC. During installation, if the current user has Administrator privileges, the installation program will automatically prompt for installation of this driver.
If the installer does not have Administrator privileges, someone with Administrator privileges will have to log in and install the driver manually. The driver installation program can be found in the /Rainbow directory of the FEMAP CD. On 32-bit Windows platforms, run CD\Rainbow\SPI722.exe. On 64-bit systems, run "CD\Rainbow\Sentinel System Driver\Sentinel Protection Installer\Sentinel Protection Installer 7.1.0.exe" It is highly recommended that you do not have any security devices attached to your computer while you are installing the driver. Once the driver has been installed, you can plug a USB security device directly into an open USB port and it should be recognized. For the Parallel Port security device, it is highly recommended that you shut your computer down and turn it off before installing the security device. After it is installed, turn the computer on begin using FEMAP.
Setup Program Execution Windows 2000/XP/Me 1. Log in to your computer as Administrator. As detailed above, this will make installation of the driver required to talk to the FEMAP dongle possible. 2. Insert the FEMAP CD into the drive. The setup should automatically begin within a few seconds. If it does not, manually run the SETUP.EXE program in the root directory of the FEMAP CD. Once setup is running you will see a license agreement. Assuming that you agree with the license agreement, press Yes to continue and select the directory where you would like to have the FEMAP program files installed. You will now be asked which type of installation to perform.
Setup Program Execution
2-3
Setup Type
Description
300-Node Demo
Installs the 300-Node demonstration version of FEMAP. This version requires no licensing, but is limited to very small models. It is intended for new users to try FEMAP and all its options.
Network Client
Network Client Installs the Network Client version of FEMAP. This setup is for use where FEMAP is licensed via the FLEXlm license management software. With the Network Client version of FEMAP, one machine on your network will be designated as the license server. The following "Network License Server" setup will have to be run on that mac
Network License Server
Installs the software required to run one computer on your network as the license server providing licenses to FEMAP client machines. The License Server machine can hand out as many licenses as you have purchased.
Stand-Alone
This is by far the most popular setup type used when installing FEMAP. It installs FEMAP for use with a Rainbow Parallel Port or USB dongle. If you have the dongle version of FEMAP, choose this setup type.
VisQ and Client and Server
VisQ is a free utility shipped with FEMAP. VisQ creates a client server environment where VisQ Server is installed on a computer that has access to FEA solver codes. VisQ Client machines can then send FEA input files to VisQ Server across the network. VisQ Server will run the analysis jobs in queue, and when each job is finished, the results are sent back to the client. For more information on VisQ, please see VisQ.PDF in the PDF directory under FEMAP.
After choosing your Setup Type, you will be prompted for the selection of additional FEMAP options, please choose any optional modules and components that you wish to have installed.
2-4
Installing FEMAP
Upgrading Your Security Device FEMAP dongles are shipped good for 30 days from the first time they are run. In order to remove the time limit from your new FEMAP dongle, or upgrade an older dongle or network license, you must contact UGS PLM's Global Technical Access Center (GTAC). In order to retrieve your FEMAP upgrade codes or your FLEXlm license file, you will need a GTAC WebKey account.
Obtaining a Webkey Account from UGS To request a WebKey account, access the web page; then provide the following information: https://plmapps.ugs.com/webkey •
Your Installation ID
•
WebKey Access Code
Your Installation ID is directly under the "sold to" information on your shipping order. For dongle-based FEMAP customers, your WebKey Access code is the unique portion of your FEMAP serial number, i.e. 3H-NT-1234, which is displayed in your current FEMAP in the Help - About dialog box, for this license as 820-3H-NT-1234, with the version information at the beginning of the serial number removed. If you have any problems determining your Installation ID, FEMAP Serial Number, or have trouble getting a WebKey account, please contact: Trish McNamara - [email protected] - 610-458-3660 x30, or Mark Sherman - [email protected] - 610-458-3660 x17
Obtaining Upgrade Codes or a new License File 1. Via the Web, using your WebKey Account -Upgrade codes or an updated license file can be e-mailed to you from the Customer Support (GTAC) web site http://support.ugs.com. Select the "License & Passwords" icon or select the "current license" option under the "License Retrieval" menu from the left side of the main GTAC screen. Select "Femap" as the Product. 9.00 as the Version, and fill in the LM Host with the unique portion of you FEMAP serial number (3H-NT-7878 in this case), or for FLEXlm network licenses, fill in the Ethernet address of your FEMAP license server. Your license will be e-mail to the address supplied during WebKey registration.
2. Via the Phone - You can call GTAC at 714-952-5444 (US and Canada residents may use 800-955-0000) and enter option 1, 1, for your CSR or option 1,2, for Software Product Delivery (SPD). You should then request a copy of the license upgrade for a specific Installation ID and serial number or Ethernet Address. For dongle versions of FEMAP, the information returned to you to upgrade the dongle will be in the form of two case insensitive alpha numeric codes. They will appear something like:
Access Code 1: 08aeca3f0f52639179 Access Code 2: 362ff63c3426d943
Use the Help, About command, then click the Security button. Cut and paste (to avoid errors) or type these two codes in to the appropriate fields and press OK. The FEMAP dongle is an EPROM, and these codes are used to update the memory of the dongle. Once these codes have been entered, you will never need to enter them again,
Network Installation - PC
2-5
with changes made to the memory of the dongle, they will either be useless, or simply write the same thing to memory again.
Network Installation - PC The “Network Client” version of FEMAP utilizes the FLEXlm License Manager software from Globetrotter Software Inc. This licensing approach requires some software to be installed on a server machine and other software to be installed on one or more clients. The clients then request and obtain licenses from the server. In a simple situation, both the client and server could be the same computer, but more likely they are different systems connected by a network.
Obtaining a License File License files are obtained through the same procedure as defined above for getting the upgrade codes for a dongle license. Call GTAC, or use your WebKey account to request your FEMAP license file. The only difference in Network Licensed FEMAP is that you need to enter the LMHostID (Ethernet Address) of your license server when prompted instead of the FEMAP Serial Number. When you receive your license file information, you need to extract just the valid FLEXlm license entries, and copy them into a file called "license.dat". Please make sure that your license.dat looks something like the one show below. For FEMAP, you will have one SERVER line, one DAEMON line, and one or more FEATURE lines depending on how many options you have purchased with your FEMAP. A couple of things to make sure of: 1. Make sure that the entry immediately following the word "SERVER" is the name of the license server where you are installing the license server software. If it is a temporary name, i.e. ANY, or THISHOST, change it to the correct machine name. This is one of the two things in the license file that you can change. 2. Make sure that the third entry on the SERVER line matches the LMHostID of license server. This number is the key to the whole license file. If this does not match the LMHostID of the license server, then the licensing will not work. 3. The "DAEMON esplmd" line calls out the actual programs that hands out FEMAP licenses. If you have installed all the license server pieces in the same directory, it is fine as is. If the esplmd.exe program is not in the same directory as LMTOOLS.EXE, you will have to edit this line to tell LMTOOLS.EXE where to find it. This is the other part of a license file that you can change. SERVER PHLF10 00095b8e20ef DAEMON esplmd FEATURE femap esplmd 9.20 18-may-2007 1 0588B50324A5 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapthermal esplmd 9.20 18-may-2007 1 DBB2754C3B21 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapadvthermal esplmd 9.20 18-may-2007 1 7033101A44B2 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapflow esplmd 9.20 18-may-2007 1 0F1D6AB8AE56 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_basic_fep esplmd 9.20 18-may-2007 1 EE2DC8632354 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_nonlin_fep esplmd 9.20 18-may-2007 1 861F50768DA3 \ VENDOR_STRING=920-FX-NT-20ef0001762070000 FEATURE femapnx_nas_dyn_fep esplmd 9.20 18-may-2007 1 8ECB283B0927 \ VENDOR_STRING=920-FX-NT-20ef0001762070000
License Server This section provides instructions on installing the network license manager and configuring your server.
2-6
Installing FEMAP
Installing the FLEXlm License Manager To begin the server installation, simply insert the FEMAP CD and allow it to AutoRun, or choose setup from the CD. When asked for the type of installation that you want to perform, select the "Network License Server" setup type. Once FEMAP has installed the software, copy your license file (usually called "license.dat") to the same directory where you installed the license server components.
Configuring the FLEXlm License Manager You can run the LMTOOLS program, from the FEMAP entry on your start -> All Programs - FEMAP v9 FLEXlm Tools, or manually run LMTOOLS.EXE from its installed directory.
Once LMTOOLS is running, select the "Config Services" Tab.
Fill in a Service Name, specify a path to the lmgrd.exe file (a required FLEXlm component) that can be found in the installation directory, and specify the path the license file. Finally, check the "Use Services" option, and then the "Start Server at Power Up". Press the "Save Service" button.
Answer "Yes" to:
You must start the license server manually the first time, press the "Start/Stop/Reread" tab.
Configuring the FLEXlm License Manager
2-7
Select the FEMAP service that you just created, and press the "Start Server" button. At this point FLEXlm will be handing out FEMAP licenses on your network. To verify that everything is working fine from the license server standpoint, press the "Server Status" tab.
Press the "Perform Status Enquiry" button and the text window will be filled with status information about your FLEXlm license server. In the text window you will find information about how many licenses are available, and once user start checking out licenses, how many are in use.
2-8
Installing FEMAP
Configuring Network Client Machines Once your network license server is up and running, configuring FEMAP Network Client machines is very easy. Make sure that FEMAP is installed on the local machine using the "Network Client" setup type. To configure client machines to access the network license: You have two options for telling network client machines how to find licenses on the license server: 1. Place a copy of the "license.dat" file in the FEMAP directory on the client machine. FEMAP will extract the name of the license server from the license file, and check out a license and run. The only drawback to this approach is that you must remember to update every copy of the license file when you receive a new one from UGS (updates, licensing changes, etc.). To avoid this problem, you can type in the full network path to the License File in the "License File" field used below for HostName/IP Address location of the license server. 2. Tell FEMAP the name or IP address of the License Server. a. Start FEMAP b. Go to Help - About - Security c. In the "License File" field, enter the name of the license server, preceded by an ampersand. In the example below, FEMAP is told to check out licenses from a network machine named PLSRV2: d. In order for this machine name approach to work, the client computer must be able to see the license server computer via TCP/IP networking. To verify this, you can open a Command Prompt and ping the license server. In this case, one would type "ping PHLSRV2". The ping command will let you know if it can talk to the machine name indicated. If the client computer cannot find the license server by its name, you can also enter the IP address of the license server, preceded by an ampersand and licensing should also work.
Monitoring Network Usage In a multi-user environment, sometimes you will not be able to get a license simply because all available licenses are in use. You can find out who is using licenses, which computers they are using and when they started their license simply by going to Help, About, and pressing the Security button. At the bottom of the dialog box you will find information that will give you this information. If you fail to get a license because none are available, you will not be able to work in FEMAP. You do not however, have to leave FEMAP. You can simply stay there and periodically try a command. Whenever a license becomes available it will be assigned to you and your command will succeed. If there are still no licenses available, you will simply get a message that says try again later.
Errors Starting FEMAP Security Device Not Found Symptom: You see an error indicating that the security device cannot be found. Resolution: Go to Section , "Security Device", and confirm all steps have been followed. Try to run FEMAP again.
Errors Starting FEMAP
2-9
Choose Server or File Symptom: If you are attempting to start a network client and see the Error dialog box from FEMAP, FLEXlm cannot find a valid license file. Resolution: Press Cancel in this dialog box. Pick Help, About, Security to define the location of the license file, as instructed above in Section , "Configuring Network Client Machines"
Unable to get license message:
LM_LICENSE_FILE environmental variable error:
This error will ONLY occur when the environment variable LM_LICENSE_FILE has been set. For example, this environment variable may have been set by another application for licensing purposes. Be careful when removing or altering this environment variable as it may cause other applications to no longer function properly.
Other Error Messages Symptom: If you receive an “Unable to allocate Scroll Buffer File” error or have any other difficulty starting FEMAP where abnormal termination occurs, you either do not have enough disk space, or your Windows TEMP is not set to a valid, accessible directory. Resolution: You may either change your Windows TEMP directory environment variable, or specify a path for the FEMAP scratch files (which default to the Windows TEMP directory set by the environment variable) to a valid directory. This and all other FEMAP preferences are stored in a file called femap.ini that is typically located in the FEMAP executable directory. You will have to create this file or modify it to include the appropriate lines as shown below: DISKMODELSCR=C:\FEMAP92 DISKLISTBUFF=C:\FEMAP92
2-10
Installing FEMAP
where C:\FEMAP90 can be any valid path. The DISKMODELSCR, DISKUNDO, and DISKLISTBUFF parameters are case sensitive, and must be defined exactly as above. Once you make these changes and FEMAP starts, you can use the File, Preferences, Database command to modify this path.
Starting FEMAP There are several command line options to launch FEMAP. The simplest method to launch FEMAP is to create a shortcut for FEMAP on your desktop and double-click the icon when you want to launch FEMAP. This will use the command line contained under the shortcut to launch FEMAP. You can modify this command line by right-clicking on the FEMAP icon, selecting properties, and changing the command line option on the shortcut. The command line will contain the executable (and its path). After the femap.exe, there are several options which may be used to determine the mode in which FEMAP will operate. A list of these command line options are provided below. c:\femap93\femap.exe [-R] [-NEU] [-NOSPL] [-D dxf_file] [-N neu_file] [-PRG program_file] [-SE Solid Edge_File] [-L port] [-SAT sat_file] [-XMT x_t file] [-SCA scale_factor] [-IGES iges_file] [model_file or ?]
where all of the arguments in [ ] are optional command line parameters. They are: The remaining parameters can be specified in any order. -R
Read Only Mode. With this option set, the Save, Save As and Timed Save commands are disabled. You will not be able to save changes to any model you access. All other commands remain active. Any changes you make will be made in the temporary scratch file, and will be lost when you exit FEMAP.
-NEU
Automatically writes a neutral file with the same name (just .NEU extension) as your .MOD file every time you save a model. In addition, when you open a model, if a neutral file exists with a newer date than the model, it will be read.
-NOSPL
Starts FEMAP without the splash screen.
-D dxf_file
This option automatically reads the specified DXF file when you start FEMAP. Make sure you leave at least one space between the two arguments.
-N neu_file
This option automatically reads the specified FEMAP neutral file when you start FEMAP.
-PRG program_file
This option allows you to run a specified FEMAP program file (*.PRO or *.PRG file) when FEMAP is started.
-SE Solid Edge_file
Automatically creates a new FEMAP file and calls the File, Import Geometry command to read the Solid Edge part file (*.prt file) or assembly file (*.asm file). When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box, which will contain the title of the solid model file contained in the SAT file.
-L port
Specifies the parallel port where the FEMAP security device has been installed. This is not typically needed unless FEMAP has difficulty accessing the device. If you want to attach the security device to parallel port 1 (LPT1:), use -L 1, for parallel port 2 (LPT2:) use -L 2. If your system is non-standard, or uses some other parallel port convention, you can specify the actual parallel port address. For example, if your parallel port was at address 03BCH (hexadecimal), you would convert the address to a decimal value, in this case 956, and specify -L 956. If you need to specify the -L option, you can change the default command line associated with the FEMAP icon on the Desktop by selecting Properties. First, right-click on the FEMAP icon. Then choose the File, Properties command (or press Alt+Enter). Move down to the command line option, and just add the appropriate -L options. From then on FEMAP will look for the security device on the specified port.
Improving Performance (RAM Management)
2-11
-SAT sat_file
Automatically creates a new FEMAP file and calls the File, Import Geometry command to read the ACIS solid model file *.SAT file [sat_file]. When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box, which will contain the title of the solid model file contained in the SAT file.
-XMT xmt_file
Automatically creates a new FEMAP file and calls the File, Import, Geometry command to read the Parasolid solid model file *.X_T file [xmt_file]. When you use FEMAP with this command option, you will see the Solid Model Read Options dialog box which will contain the title of the solid model file contained in the X_T file.
-SCA scale_value
This option is used in conjunction with the -XMT and -SAT to specify a scale factor for the solid model. If this option is used, FEMAP will automatically import and scale the solid model. The Solid Model Read Options dialog box will not be shown.
-IGES iges_file
Automatically creates a new FEMAP file and calls the File, Import, Geometry command to read the file [iges_file]. When you use FEMAP with this command option, you will see the IGES Read Options dialog box, where you can specify options for reading the file.
model_file
Normally FEMAP will start with a new, unnamed model. If model_file is the filename of an existing model however, FEMAP will start using that model. If the file does not exist, you will see an error message, and FEMAP will start a new model with that name.
?
If you add a question mark to the command line instead of specifying a model name, FEMAP will automatically display the standard file access dialog box and ask you for the name of the model that you want to use. If you want to begin a new model, just press New Model or the Escape key. When you want to work on an existing model, just choose it from the dialog box, or type its name. You should never specify both the ? and model_file options.
Improving Performance (RAM Management) To improve FEMAP performance on Windows personal workstations, you should modify the default settings that FEMAP uses to manage RAM. For more details on this procedure, see Section 2.6.2.5, "Database" in FEMAP Commands. To access the internal FEMAP memory management system, follow the procedure below: 1.Choose the File, Preferences command and click the Database tab. 2.Change Cache Pages and Blocks/Page in the dialog box. 3.Set Max Cached Label to a number that is higher than any entity you will create in your model file. This sets aside a small portion of memory that stores all of the IDs in FEMAP. 4. Select OK The total amount of memory that FEMAP can allocate is the product of the Cache Pages, Blocks/Page, and 4096 bytes/ block. For example, with the values shown, 12000 x 2 x 4096 will allow FEMAP to access just under 100 Mbytes of RAM and use entity ID’s up to 6,000,000. Note: You should never allow FEMAP to allocate more than the physical memory of the machine. The internal memory management (swapping) in FEMAP will allow the program to run much faster than Windows memory swapping. Therefore, you should set the Cache Pages and Blocks/Page at a level which is comfortably below the physical memory of the machine. Also, to optimize performance, you should always increase Cache Pages (max 15000) to its limit before increasing Blocks/Page.
2-12
Installing FEMAP
Memory Setting Guidelines The following figures are provided as a starting point to improve performance. Operating System
Installed RAM (Mb)
Windows 2000, Me, 64 XP 128 256 512 1000
Cache Pages 6000 8000 12000 15000 15000
Blocks/Page 1 2 3 5 11
Actual performance will vary depending upon other concurrent applications and model specifics. It is best to increase Cache Pages to 15000 before increasing Blocks/Page. Note: For best performance, you should have enough physical RAM to load the entire model file into memory. For example, if you expect your model files to be a maximum of 100 Mb, then you would want FEMAP to allocate at least 100 Mb of memory. If you had 128 Mb of physical RAM, this would leave 28 Mb for Windows and other programs that may be running at the same time as FEMAP.
Licensing Conversion Methods Please read this section very carefully before changing your licensing method. If you are going to convert your licensing method you MUST HAVE FEMAP AND NX NASTRAN CLOSED (not running) before you use the files described below. You can change your licensing method (i.e., from using a security key to using a network license) using specific “batch” files located in the FEMAP directory. The files are named “go_licensing method”.bat and require minimum user input to change your licensing method. In general, the “go” batch files change your current “auth_92.dll” to use the appropriate licensing method (auth_licensing method.dll) and may create or alter some other required files. FEMAP will open a “command prompt” and let you know if the conversion of the auth_92.dll has been successful. The various “go” files are explained in greater detail below: •
go_apionly.bat - converts your current licensing method to the “API Only” version of FEMAP
•
go_demo.bat - converts your current licensing method to the FEMAP 300-Node Demonstration version.
•
go_dongle.bat - converts your current licensing method to use a security key.
•
go_network.bat - converts your current licensing method to use the FlexLM Network Client.
3.
Analyzing Buckling for a Bracket
In this first example, you will explore the buckling load of a simple bracket subject to a concentrated cantilevered load. The bracket, although solid, will be idealized as a thin shell finite element model, fixed at the base and loaded at the tip.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the bracket
•
meshing the model
•
applying constraints and loads
•
analyzing the model using the NX Nastran solver
•
post-processing the results
Importing the Geometry What Import a FEMAP neutral file containing the geometry of the bracket.
How Step
UI
Command/Display
1.
File, New Menu
2.
File, Import, FEMAP Neutral Menu
3-2 Step
UI
Analyzing Buckling for a Bracket
Command/Display
3.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory in your FEMAP installation.
4.
File name: Bracket.NEU Open Neutral File Read Options dialog box: OK
V1
ZX Y
Meshing the Model The first step for the meshing process will be to define the property and material for the elements. Next, you will mesh the surfaces.
Defining the Property and Material The shell property represents the thickness of the material making up the two regions of the part.
What Define the shell element property.
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Elem/Prop Type
3.
Element/Property Type dialog box: Plane Elements: Plate OK
Meshing the Model
Step 4.
UI
3-3
Command/Display Define Property dialog box: Title: Shell Notice: Titles can be up to 79 characters long in FEMAP 9.3 and above
5.
Property Values: Thicknesses: 0.1
6.
OK Yes (to create material) Notice: You have created the property, but you also need to define the associated material. In steps below, you will choose a standard material from the FEMAP material library.
7.
Define Material - ISOTROPIC dialog box: Load
8.
Select from Library dialog box: AISI 4340 Steel (select)
9.
OK, then... In Define Material - ISOTROPIC dialog box: OK, then... In Define Property dialog box: OK Cancel Tip: Once you defined the first property, FEMAP automatically prompted you to enter another property. To end the command, press Cancel. Generally, you will need to press Cancel to exit from any entity creation command.
Meshing the Model The geometry that you imported is simply a wireframe representation of the part’s midsurfaces. To create finite elements in FEMAP, you need to specify the regions, or “boundaries” where you need to mesh. You also need to specify how many elements that you want along the edges of a region. By default, all geometry is assigned a mesh spacing of 1.0. If you mesh this part without specifying a tighter mesh size, your mesh will be too coarse to give meaningful answers. By default, you have been viewing the model in the regular wireframe mode. Once you have created the mesh, you will change to the Free Edge model style to ensure that the part is meshed continuously. Since it isn’t, you’ll use the Coincident Nodes check to merge duplicate nodes at the split between the two regions.
What Create boundary surfaces for both regions of the model.
3-4
Analyzing Buckling for a Bracket
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select the four curves that make up one of the regions (see figure below). OK
3.
Select the four curves that make up the part’s other region. OK Cancel (to end the command)
Notice: You should now have two new boundary surfaces.
V1
ZX Y What Specify the mesh size for the surfaces.
Meshing the Model
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
2.
Entity Selection dialog box: Select All OK
3.
Automatic Mesh Sizing dialog box: Element Size: 0.3 OK Cancel
What Mesh the surfaces.
How Step
UI
Command/Display
1.
Mesh, Geometry, Surface Menu
2.
Entity Selection dialog box: ID: 1 OK
3.
Automesh Surfaces dialog box: Property: Shell OK
4.
Mesh, Geometry, Surface Menu
5.
Entity Selection dialog box: ID: 2 OK
3-5
3-6 Step
UI
6.
Analyzing Buckling for a Bracket
Command/Display Automesh Surfaces dialog box: OK
ZX Y What Display the model using the Free Edge style.
How Step
UI
Command/Display
1.
F5 key
View Select Tip: You can also press the View Select icon (on the toolbar) or View, Select command to open the dialog box.
2.
View Select dialog box: Model Style: Free Edge OK
V1
ZX Y Notice: The model is displayed with only the free edges showing. As expected, there are free edges around the outside of the part. There are also free edges where the part needs to be connected, at the split line between the two regions. This indicates that there are duplicate nodes at these locations, each connected to shell elements on one side of the edge. Tip: If you had selected all the surfaces and meshed them together, the meshes on the two surfaces would have been connected.
Meshing the Model
3-7
What Check for coincident nodes, and merge them.
How Step
UI
Command/Display
1.
Tools, Check, Coincident Nodes Menu
2.
Entity Selection dialog box: Select All OK
3.
Check/Merge Coincident dialog box: Options: Merge Coincident Entities OK Notice: You will notice on the Check/Merge Coincident dialog box that a “Preview Coincident” option exists. When this option is checked, FEMAP will enter a mode which allows you to highlight the nodes which will be “Kept”, “Merged”, or “Both” in your model. Clicking “Done” will complete the operation with the selected options (i.e., listing the coincident nodes to the Messages pane, Merging the nodes, creating the appropriate groups)
4.
Window, Regenerate Menu
V1
ZX Y 5. 6.
F5 key
View Select View Select dialog box: Model Style: Draw Model OK
3-8 Step
Analyzing Buckling for a Bracket
UI
Command/Display
V1
ZX Y
Applying Constraints and Loads Next, you will apply constraints and loads to the model. Since most parts and systems of parts can be held and loaded in any number of ways, FEMAP uses sets to manage constraints and loads. First, you will create a constraint set, then you will fix all of the nodes at the base of the model. Next, you will create a load set, then apply a 100 pound load to the tip of the bracket. In a buckling analysis, the actual loading of the part is applied, and the solver returns a buckling eigenvalue. The eigenvalue is multiplied by the applied load to give the critical buckling load.
Applying Constraints What Create the constraint set.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
What Create the constraints to fix the nodes at the base of the model.
Applying Constraints
How Step
UI
Command/Display
1.
Model, Constraint, Nodal Menu
2.
Entity Selection dialog box: Pick the nodes at the edge of the model. OK
3.
Create Nodal Constraints/DOF dialog box: Fixed OK Cancel
V1 C1
ZX Y 4. 5.
Ctrl-Q keys
123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456 123456
View Quick Options View Quick Options dialog box: Labels Off Done
3-9
3-10 Step
Analyzing Buckling for a Bracket
UI
Command/Display
V1 C1
ZX Y
Applying Loads Apply the 100-pound load to the model.
What Create the load set.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Title: (enter a title) OK
What Create the load in the negative Y direction.
How Step
UI
Command/Display
1.
Model, Load, Nodal Menu
2.
Entity Selection dialog box: Pick node at the tip of arrow (see following figure). OK
Analyzing the Model
Step
UI
3-11
Command/Display
V1 C1
A
ZX Y 3.
Create Loads on Nodes dialog box: FY: Value: 100 Notice: The default load type is force.
4.
Click OK, then... Click Cancel
V1 L1 C1
ZX Y
Analyzing the Model The FEMAP analysis manager stores the options for creating an input file for a solver (an analysis set). It can launch the NX NASTRAN solver or another solver that has been set up to run on the same PC. The analysis manager, together with VisQ, can also set up and run analyses with solvers on other PCs. The analysis sets are stored with the FEMAP model file, and can also be stored in a FEMAP library that can be accessed from different model files.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
3-12 Step
UI
Analyzing Buckling for a Bracket
Command/Display
2.
Analysis Set Manager dialog box: New
3.
Analysis Set dialog box: Title: Buckling
4.
Analysis Program: 36..NX Nastran Analysis Type: 7..Buckling
5.
Click OK
Notice: The analysis set manager displays all analysis sets defined in the model, and the sections that make up the input file for the solver. Clicking on a plus sign will expand the tree and display individual options that can be edited by double-clicking on an option. For this analysis, you’ll use the default values for these options. 6.
Analyze
Notice: The Graphics window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results For this example, you will display the buckling shape and buckling factor.
What Display the deformed model (buckled shape) and the critical buckling factor.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: Deform
3.
Deformed and Contour Data
Post-processing the Results
Step 4.
UI
3-13
Command/Display Select PostProcessing Data dialog box: Output Set: 2..Eigenvalue 1 33.02924 OK (all dialog boxes)
Notice: The set value is the eigenvalue and critical buckling factor for a buckling analysis. In this case, the part would buckle at a load 33.03 times higher than the applied load. This is the end of the example. You don’t need to save the model file.
3-14
Analyzing Buckling for a Bracket
4.
Creating and Meshing a Solid Model In this example, you will use the FEMAP geometry modeling capabilities to build a solid model of a slotted guide. You’ll apply constraints and loads, then mesh the model.
1
To perform this example, you’ll need to have the Parasolid modeling engine active. If you have the 300-node version of FEMAP, you won’t be able to save your model file or change the model after meshing due to size limitations. Y Z
X
The example includes the following steps: •
importing the geometry
•
creating the solid part
•
creating the slot
•
creating the bolt holes
•
creating the guide boss
•
applying constraints and loads
•
meshing the model
Importing the Geometry What Open a new model file and import the FEMAP neutral file containing the basic profile for the part.
How Step
UI
Command/Display
1.
File, New Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory.
4-2 Step
UI
Creating and Meshing a Solid Model
Command/Display
4.
File name: Slot.NEU Open
5.
Neutral File Read Options dialog box: OK Notice: The imported curves will form the base of the part.
V1
Y ZX
Creating the Solid Part To create the part, you’ll first create a boundary, then extrude it.
What Create a boundary from the curves.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select All OK Cancel
What Extrude the boundary to form a solid part.
Creating the Solid Part
4-3
How Step
UI
Command/Display
1.
Geometry, Solid, Extrude Menu
Notice: Since there is only one boundary, the software selects it automatically. 2.
Material: New Solid Direction: Negative Length: To Depth
3.
To Depth: 10 OK
4.
Dynamic Rotate (on View Toolbar)
5.
Dynamic Display dialog box: Hold the left mouse button and rotate the model to see the extrusion. OK Tip: If you are in Render mode, you do not have to pick the Dynamic Rotate icon on the toolbar before using the mouse to dynamically rotate your model. Render mode is the default graphics mode and uses the OpenGL graphics language. Render mode can only be turned off by using the View, Options command. Once the View Options dialog box is open, select Tools and View Style in the Category section, then select Render Options from the list of Options. Click the Graphics Engine button and select Windows GDI in the dialog box, then Click OK and OK again. There is NO reason to turn off Render mode when doing the Examples.
6.
Click OK when you are done rotating the model.:
V1
Y Z X
4-4
Creating and Meshing a Solid Model
Creating the Slot What To start drawing the slot, create two circles.
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
2.
Locate dialog box: 0, 95, 0 (enter these X, Y, Z values for the center of the circle) OK
3.
11, 95, 0 (enter a point on the circle) OK Notice: FEMAP prompts you to create another circle.
4.
Define another circle: 0, 50, 0 (center), Click OK, then... 11, 50, 0 (point on the circle), Click OK, then Cancel
V1
Y ZX What Finish creating the geometry of the slot.
Creating the Slot
4-5
How Step
UI
Command/Display
1.
Geometry, Curve - Line, Points Menu
2.
Create Line from Points dialog box: Pick points A and B. OK
V1 C
A A
D
B
Y ZX 3.
Create another line from points C to D. Click OK, then Cancel
V1
Y ZX What Break the circles into 2 parts.
How Step 1.
UI
Command/Display Snap to Point can be found on Select Toolbar snap modes menu or from on the Quick Access Menu (click right mouse button in graphics window) Tip: The snap modes can also be chosen using the “Right Mouse Menu” in FEMAP. Simply right-click the mouse in the graphics window and choose the appropriate snap option.
4-6 Step
UI
Creating and Meshing a Solid Model
Command/Display
2.
Modify, Break Menu
3.
Entity Selection dialog box: Pick the lower circle. OK
4.
Locate dialog box: Pick point A (in following figure). OK Tip: You need to check that the view axes are oriented the same as in the following figure. If the model is reversed and you pick the points opposite A and B, you will be picking the end point of the circular curves and the split will fail.
V1 B
A
Y ZX 5.
Pick the upper circle, then break it at point B.
6.
Delete, Geometry, Curve Menu
7.
Entity Selection dialog box: Pick the two inner halves of the circles.
Creating the Slot
Step
UI
4-7
Command/Display
8.
OK Yes (delete the curves) Tip: The Update Views check box on the Confirm Delete dialog enables you to automatically regenerate the graphics after the deletion. If you are doing a lot of deletes in a large model, you might want to uncheck this box to improve performance and then press Ctrl-G to regenerate the display when you have finished deleting entities
V1
Y ZX What Create a boundary surface and extrude the new curves.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Pick the four curves of the slot. OK, then... Cancel
4-8 Step
UI
Creating and Meshing a Solid Model
Command/Display
3.
Geometry, Solid, Extrude Menu
Notice: The boundary that you just created is already selected. 4.
Extrusion Options dialog box: Material: Remove - Hole Direction: Negative Length: Thru All OK
V1
Y Z X
Creating the Bolt Holes You’ll now use a patterning technique to create five bolt holes.
What Use a pattern to create five bolt holes.
Creating the Bolt Holes
4-9
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
-38, 0, 0 (center), Click OK, then... -38, 5, 0 (a point on the circle), Click OK, then... Cancel
V1
Y ZX 2.
Geometry, Boundary Surface, From Curves Menu
Pick the circle. OK, then Cancel 3.
Geometry, Solid, Extrude Menu
4.
Extrusion Options dialog box: Material: Remove Hole Direction: Negative Length: Thru All Tip: Make sure that the Extrude arrow extends through the thickness of the part. If it points the wrong way, change the Direction.
5.
Pattern
6.
Patterns dialog box: Radial
7.
Center: 0, 0 (XY coordinates) Number: 5 Total Angle: 180 OK (all dialog boxes)
4-10 Step
UI
Creating and Meshing a Solid Model
Command/Display
V1
Y ZX
Creating the Guide Boss Next, create the guide boss and its slot.
Creating the Guide Boss What Create the geometry of the guide boss.
How Step
UI
Command/Display
1.
Geometry, Curve - Circle, Radius Menu
2.
For the first circle, enter: 0, 0, 0 (center) 25, 0, 0 (point on circle)
3.
For the second circle, enter: 0, 0, 0 (center) 16, 0, 0 (point on circle)
4.
Zoom (on View Toolbar) Pick two corners to draw a box around the two new circles.
Creating the Guide Boss
Step
UI
4-11
Command/Display
V1
Y ZX 5.
Geometry, Boundary Surface, From Curves Menu
Select the two new curves. OK 6.
Geometry, Solid, Extrude Menu
7.
Extrusion Options dialog box: Material: Add - Protrusion Direction: Positive Length: To Depth
8.
To Depth: 50 OK Tip: To better see the model, rotate it and change to a solid model display: pick the View Style icon on the View Toolbar, then pick Solid. To restore the display, pick View Style, then pick Wireframe.
4-12
Creating and Meshing a Solid Model
Creating the Guide Boss Slot Create the slot in the guide boss.
What Move the workplane to the top of the boss, so that you can more easily build the slot. The workplane is a two-dimensional plane that you can locate and align anywhere in three-dimensional space. When you make a graphical selection, the screen location that you selected is projected along a vector normal to the screen onto the workplane. The resulting three-dimensional coordinates are located at the intersection of the projection vector and the workplane. How Step
UI
Command/Display
1.
Tools, Workplane Menu
2.
Draw Workplane (check)
3.
On Surface
4.
Plane Normal to Surface dialog box: On Surface: (pick the surface highlighted below) At Point: (pick point A) Axis Point: (pick point B) OK
A
B
What Create the boss slot. First, you’ll create a horizontal line on the surface of the boss. Next, you’ll create two parallel lines, and use them to form a rectangle. Finally, you’ll extrude the rectangle to create the slot.
Creating the Guide Boss Slot How Step
UI
Command/Display
1.
Geometry, Curve - Line, Points Menu
2.
Create Line from Points dialog box: From Point: (pick point A from previous diagram) To Point: (pick point B) OK Notice: There is a new horizontal line on the surface of the guide boss.
V1
Y ZX 3.
Geometry, Curve - Line, Parallel Menu
4.
Line Parallel to a Line dialog box: From Curve: (pick the curve you just created) Offset: 3.5 OK
5.
Locate dialog box: Pick a point to one side of the line, such as point A below. OK
4-13
4-14 Step
UI
Creating and Meshing a Solid Model
Command/Display B
V1
Y ZX 6.
A
Pick the line again. Pick a point on the other side of the line, such as point B above.
Notice: The guide boss now has three parallel lines on the top.
V1
Y ZX 7.
Geometry, Curve - Line, Points Menu
8.
Create Line from Points dialog box: From Point: Pick point A (the endpoint of the top line) in the following diagram. To Point: Pick point B. OK
V1
A
C
B
D
Y ZX
Creating the Guide Boss Slot
Step
UI
Command/Display
9.
Create another line between points C and D.
10.
Geometry, Boundary Surface, From Curves Menu
11.
Pick the four curves below to form a rectangle.
V1
Y ZX 12.
Geometry, Solid, Extrude Menu
13.
Extrusion Options dialog box: Material: Remove - Hole Direction: Negative Length: To Depth
14.
To Depth: 12 OK
4-15
4-16
Creating and Meshing a Solid Model
Applying Constraints and Loads For constraints, fix the bolt holes. Next, create a load on the inner surface of the slot.
What Create a constraint set, then apply constraints to the bolt holes.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
3.
Model, Constraint, On Surface Menu
4.
Entity Selection dialog box: Pick the 10 inner surfaces of the bolt holes. OK
5.
Create Constraints on Geometry dialog box: Fixed OK
Applying Constraints and Loads
Step
UI
Command/Display
V1 C1
Y ZX 6.
Ctrl-A
Autoscale the model (display the entire model in the Graphics window).
V1 C1
Y Z X What Create the load set, then apply a load of -1000 pounds to one face of the slot.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Title: (enter a title) OK
3.
Model, Load, On Surface Menu
4-17
4-18 Step 4.
UI
Creating and Meshing a Solid Model
Command/Display Entity Selection dialog box: Pick one face inside the slot (see the following figure). OK
Tip: Rotate and zoom the model so that you can more easily see the face. 5.
Create Loads on Surfaces dialog box: FX: Value: -1000 OK
V1 L1 C1
Y ZX
Meshing the Model Define the property and material for the model, then generate a solid mesh.
Defining the Property and Material What Define the solid element property.
Defining the Property and Material
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Elem/Prop Type
3.
Element Property Type dialog box: Volume Elements: Solid OK
4.
Title: Solid OK Notice: Titles can be up to 79 characters long in FEMAP 9.3 and above
5.
Yes (to create material)
6.
Define Material - ISOTROPIC dialog box: Load
7.
Select from Library dialog box: AISI 4340 Steel (select)
8.
OK (all dialog boxes), then... In Element Property Type dialog box: Click Cancel
What Create a solid mesh for the model.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Automesh Solids dialog box: OK
4-19
4-20 Step
UI
Creating and Meshing a Solid Model
Command/Display
V1 L1 C1
Y Z X This is the end of the example. You don’t need to save this model file.
5.
Working with Groups and Layers
The FEMAP group and layer capabilities enable you to segment your model into smaller, more manageable, discrete pieces. You can then use these pieces to minimize the amount of information displayed in the Graphics window or included in a printed report. Groups and layers also make it easier to manipulate, update, and apply loads to your model. This example introduces groups and layers. •
FEMAP groups identify portions of your model. Once you create a group, you can limit your display to the portion of the model that is in the group. In addition, a group can impact post-processing. For instance, FEMAP can automatically adjust contour/criteria limits to the peak values that occur on the entities in the group. You can also easily group elements using a particular property or material.
•
FEMAP layering is similar to layering in most CAD systems. In FEMAP, you can think of a layer as a clear sheet of “paper” with entities drawn on it. The display of the model may include many layers overlaid on one another. You can control which entities are displayed by defining which layers are visible.
Other FEMAP capabilities that control how the display of your model include the View - Select and View - Options menus, as well as post-processing displays. These features are explored in other examples.
Differences Between Groups and Layers Both groups and layers enable you to control the display of your model. However, there are some key differences between groups and layers:
Groups
Layers
An entity can be included in multiple groups.
An entity can be included in only one layer.
Only one group can be displayed at a time.
Multiple layers can be displayed at the same time.
Only one group can be active. (You can only work with one group at a time.)
Only one layer can be active. (You can only work with one layer at a time.)
See Also •
Section 5.9.2, "Groups and Layers Overview" in the FEMAP User Guide
•
Section 6.4, "Groups and Layers" in FEMAP Commands
Using Groups In this series of examples, you’ll use the wing model to create and work with several different groups.
Creating a Group What Open the model file containing the wing model. Change the view style to quick hidden line, and turn off the display of loads and constraints.
5-2
Working with Groups and Layers
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Wing.MOD file.
V1 L1 C1
Y Z X 3.
File, Save As Menu
Save the model file with a different name. 4.
View Select (on View Toolbar)
5.
View Select dialog box: Model Style: Quick Hidden Line OK
6.
Quick Options (on View Toolbar)
7.
View Quick Options dialog box: Load/Constraint Off Done
Creating a Group
Step
UI
5-3
Command/Display
V1 L1 C1
Y Z X What Create a group that represents just the upper and lower wing skins.
How Step
UI
Command/Display
1.
Group, Set Menu
Tip: You can also create a new Group using the New command on the “context sensitive menu” located on the Groups branch in the Model Info tree (simply click to highlight the top level of the Groups branch or any existing Group, then right mouse click to see the context sensitive menu). 2.
Create or Activate Group dialog box: Title: Wing Skins OK
3.
Group, Element, Property Menu
4.
Entity Selection dialog box: Pick one plate element from the top wing skin (property 101). Pick one plate element from the bottom wing skin (property 102). Rotate the model if necessary. OK Notice: As you select elements on the screen, FEMAP extracts the element’s property and fills the selection box accordingly.
What Display the new group.
5-4
Working with Groups and Layers
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Group: Select Tip: For a shortcut to the Model Data command, right-click in the Graphics window. From the menu, pick Model Data.
4.
Wing Skins (pull down menu and pick) OK (all dialog boxes)
Using a Group to Trim a Report In this next section of the example, you’ll see how groups can be useful in creating a report. Perhaps you are interested in finding the element in either the upper or lower wing skin with the maximum shear flow (FXY force). You’ll use the wing skin group to find this element.
What Create the report based on the wing skin group.
How Step
UI
Command/Display
1.
List, Output, Standard Menu
Using a Group to Trim a Report
Step
UI
5-5
Command/Display
2.
Entity Selection dialog box: OK
3.
List Formatted Output dialog box: Title: Maximum Shear Flow
4.
Sort Field: 7208: Plate XY Membrane Force
5.
Top N: Top
6.
Number: 5
7.
Format ID: 8..NASTRAN QUAD4 Forces
8.
Options: Details Only OK
9.
Entity Selection dialog box: Group: Wing Skins OK Notice: The report appears in the Messages dockable pane.
10.
Ctrl - U
Notice: Ctrl-U undocks the Messages dockable pane. The report lists the plate element forces corresponding to the top five shear flow plates in the upper and lower wing skins. The report is sorted in ascending order. You can now easily see that the maximum shear flow (FXY) is 62.31 lb./inch, and is in element 120.
11.
Ctrl - U
(Toggle back to the regular view style.)
What Quickly find element 120.
How Step
UI
Command/Display
1.
Window, Show Entities Menu
5-6 Step
UI
Working with Groups and Layers
Command/Display
2.
Entity Show dialog box: Entity Type: Element OK
3.
Entity Selection dialog box: ID: 120 OK Notice: Element 120 is temporarily highlighted.
Tip: As you’ve just seen, a group can be used in the standard entity selection box. Any time FEMAP prompts you to select entities, you can specify a group. This feature can be extremely useful when you are applying loads to a portion of your model, or when you want to update sections of your model.
Automatically Generating Groups Once you become proficient in FEMAP, you’ll probably find yourself creating groups as you build a finite element model to keep important areas of the model together for use downstream. If you don’t do this, or if you import an existing model, FEMAP has several tools for automatically grouping together portions of your model based on changes in material properties, element properties, or even geometric regions. This example shows you how to automatically split the wing mode into groups based on properties.
What Automatically generate groups based on properties.
How Step
UI
Command/Display
1.
Group, Operations, Generate Property Menu
2.
Entity Selection dialog box: Select All OK
Using the Group Information
Step
UI
5-7
Command/Display Notice: You’ve just created groups of elements based on the nine different properties in this model.
3.
Model Data
4.
Group: 2..Property 1: Upper Angle Stiffener OK Notice: The stiffeners group is displayed. If you would like “toggle on” the cross-sections of line elements and/or the thickness of plate elements for viewing, select Thickness/Cross Section from the View Style menu located on the View Toolbar
5.
Use the Model Data dialog box to display each of the other groups. Tip: You can use the Model Info tree to quickly switch the group currently being viewed. Simply expand the Groups branch so all the groups in the model are visible in a list. Highlight any group in the list and then click the right mouse button to access the “context sensitive menu” for Groups. Selecting View Active from the menu will change the view so only the “Active” group is visible. You can change the “Active” group by double-clicking on any other group in the list (the title of the group will go from black to blue text to signify the group is now “Active”). Set Model Data to Group:None in this model to use this method. Tip: You can “combine” groups very easily using the Model Info tree. Select any number of groups using the Ctrl or Shift keys and the mouse. Once the groups are selected, right mouse click and choose the Combine command. This will place all of the entities of the selected groups into one new group which can then be made “Active” to be viewed. Tip: Other than Combine, there are 5 other “boolean operations” which can be used to create new groups from multiple groups via the Group, Operation, Boolean command.
Using the Group Information In this section of the example, you’ll use a group to display specific information about the model.
What Display the axial forces in the upper stringers.
5-8
Working with Groups and Layers
How Step
UI
Command/Display
1.
Model Data
2.
Group: 6..Property 5 - Upper Stringer - T Section OK
3.
View Select (on View Toolbar)
4.
View Select dialog box: Contour Style: Criteria
5.
Deformed and Contour Data
6.
Select PostProcessing Data dialog box: Output Vectors: Contour: 3022..Beam EndA Axial Force OK (all dialog boxes) Notice: FEMAP now displays a criteria plot of the axial forces for the elements displayed.
Using Layers
5-9
Using Layers Working with layers is quite easy as long as you understand the basic layering concepts: every entity in FEMAP references a layer, and a layer is either on or off. The View, Layers command controls which layers are displayed. This section of the example shows you how to work with layers.
What Reset the display of the wing model.
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Contour Style: None
3.
Model Data
4.
Group: None OK (all dialog boxes)
V1 L1 C1
Y Z X What View the different layers in the model.
How Step
UI
Command/Display
1.
View, Layers Menu
Tip: You can also pick the Layers icon on the toolbar.
5-10 Step 2.
UI
Working with Groups and Layers
Command/Display Layer Management dialog box: Show Visible Layers Only
3.
Hidden Layers: 2..Middle Section
4.
Show
5.
Visible Layers: 1..Inner Section
6.
Hide
7.
Hide the Outer Section layer. OK
V1 L1 C1
Y Z X 8.
Layers (on View Toolbar)
9.
Layer Management dialog box: Make the following layers Hidden: Construction Layer, 2..Middle Section. Make the following layers Visible: 1..Inner Section, 3..Outer Section. OK Tip: You can “hide and show” layers very easily using the Model Info tree. Select any number of layers using the Ctrl or Shift keys and the mouse. Once the layers are selected, right mouse click and choose the Make Visible or Make Hidden commands. You can also choose to Show All Layers or Show Visible Layers Only by selecting those commands from the “context sensitive menu” for Layers
Using a Contour Group for Post-processing
Step
UI
5-11
Command/Display
V1 L1 C1
Y Z X 10.
Layers (on View Toolbar)
11.
Layer Management dialog box: Show All Layers OK
V1 L1 C1
Y Z X
Using a Contour Group for Post-processing Sometimes you may want to create an image that displays the results on a single group of elements while showing the rest of the model as a “reference”. This can be accomplished by setting a “Contour Group” in the Contour Options dialog box.
What Choose a “contour group” in the contour options dialog box.
How Step
UI
Command/Display
1.
View Select (on View Toolbar)
2.
View Select dialog box: Contour Style: Contour
5-12 Step
UI
Working with Groups and Layers
Command/Display
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Contour: 7033..Plate Top VonMises Stress
5.
Contour Options
6.
Select Contour Options dialog box: Contour Group: Select
7.
Group: 7..Property 101 - Upper Wing Skin
8.
OK (all dialog boxes)
This is the end of the example. You don’t need to save the model file.
6.
Working with View Select and View Options
FEMAP provides a wide variety of viewing options that help you be more productive. This example introduces two dialog boxes that control how your model is displayed on the screen: View Select and View Options. •
View Select controls the top level display options. With View Select, you can control whether your model is displayed in hidden line or plain wireframe mode, turn on and off stress contours, animations, deformed plots, etc.
•
View Options provides the detailed control over how entities are displayed: element color, node label display, perspective, etc. View Options also provides extensive control over post-processing options.
Other FEMAP capabilities that control how the display of your model include groups, layers, and post-processing displays. These features are explored in other examples.
Using View Select The View Select dialog box lets you control the following types of view information: •
XY Style: Controls XY plot appearance.
•
Model Style: Controls general model display.
•
Deformed Style: Controls display of deformed plots for post-processing.
•
Contour Style: Controls display of contour plots for post-processing.
The following example lets you explore some of the Model Style options. You will explore the other types of view information in the post-processing examples. For more information on View Select, see: •
Section 5.9, "Groups, Layers and Viewing Your Model" in the FEMAP User Guide
•
Section 6.1.5, "View, Select and View, Options" in FEMAP Commands
•
Section 8.2, "Types of Views - View Select..." in FEMAP Commands
What Open the model file containing the wing model.
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory.
6-2 Step
UI
Working with View Select and View Options
Command/Display Filename: Wingpost.MOD Open
V1 L1 C1
Y Z X 3.
Save the model file with a different name. Tip: Use File, Save As.
What Explore Hidden Line options.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Full Hidden Line OK Notice: Full Hidden Line shows only the entities that are visible. In Render mode, Full Hidden Line and Quick Hidden Line are the same. In non Render mode, Full Hidden Line is more accurate than Quick Hidden Line, but is slower to display.
V1 L1 C1
Y Z X
Using View Options
6-3
What On the View Select dialog box, you can use the Model Data button to control the display of load sets, constraint sets, groups, and functions. In this example, you’ll display the second load set in the model.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Load Set: Select
4.
Pressure Distribution OK (all dialog boxes) Notice: The pressure load set is now visible. Rotate the model for a better view.
C1
Y Z X 5.
View Select (On View Toolbar) dialog box: Under Model Data, select the Wingtip Loading load set. Don’t close the model file yet. You will use it in the next part of the example.
Using View Options The View Options dialog box lets you control the following categories of view information: •
Labels, Entities, and Color: Controls the display of model entities, such as nodes and elements. You can choose whether entities will be drawn, if and how they will be labeled, and the colors that will be used.
•
Tools and View Style: Controls display of tools, such as the workplane. This category also lets you control the style of the settings for free edge, element filling, shading, and perspective options. Additional options let you control view-related items such as the legend, origin, and view axes.
•
Post Processing: Controls all of the graphical post-processing options, including deformed, contour, criteria, and XY plots. None of these options, however, will have any effect unless you select one of the post-processing options through View Select.
In this example, you’ll explore the first two categories on the View Options dialog box. For more information on View Options, see:
6-4
Working with View Select and View Options
•
Section 6.1.3, “View Select and Options” in FEMAP Commands
•
Section 8.3, “View Options: Postprocessing” in FEMAP Commands
What Display the elements based on their property color.
How Step
UI
Command/Display
1.
View, Options Menu
2.
View Options dialog box: Labels, Entities, and Color (select)
3.
Options: Element (select)
Notice: The options on the right side of the dialog box change. 4.
Color Mode: 3..Property Colors (select) Apply (don’t press OK)
Notice: Press Apply to see the effects of the change without exiting the dialog box. Initially, elements are displayed based on their own (entity) color. When you change the display to Property Colors, FEMAP displays each element using the element property’s color. This capability is very useful for visualizing how the various properties in your model are distributed, and to help you ensure that elements reference the appropriate properties. 5.
You can rotate the model using the mouse while pressing the middle mouse button. If you do not have a three button mouse, press the Dynamic Rotate icon in the toolbar.
Using View Options
6-5
What Shrink the elements to make the borders of the properties easier to see.
How Step
UI
Command/Display
1.
Category: Tools and View Style
2.
Options: Shrink Elements
3.
Option On (check) Apply
Tip: In the Options list, you can double-click on the option name to toggle it on and off.
What Display the elements filled in.
How Step
UI
Command/Display
1.
Options: Fill, Backspace, and Hidden
2.
Fill On (check) OK Notice: The model is now displayed with the elements filled with their property colors.
6-6 Step
UI
Working with View Select and View Options
Command/Display
Notice: All of the options explained in the Using View Options section of this example (and more) are also available from the View Style menu located on the View Toolbar:
For instance, to quickly change the Color Mode from “Entity” to “Property” Color, choose the Color With... (Entity Colors/Property Colors/Material Colors) command on the View Style menu. In addition, the Fill and Shrink commands on the View Style menu will perform the same operations used in this example. This is the end of the example. You don’t need to save the model file.
7.
Using Post-Processing
Once you have obtained results from an analysis, you can view these results either graphically or as reports. FEMAP graphical post-processing includes deformation plots, contour/criteria plots, XY plots, and freebody plots. The graphical results can be displayed on the screen or output as a file. Report-based post-processing provides text output of post-processing data with a variety of formats, printing options, and sorting options. In this set of examples, you will explore the following FEMAP graphical post-processing capabilities: •
Deformation and contour results: You will select contour options as well as display dynamic isosurfaces and cutting planes.
•
XY plots: You will generate an XY plot of results and also generate a new results vector.
•
Results displays in other applications. You will use a deformation/contour plot in a word processing application, and an animation in a presentation application.
For more information on post-processing, see: •
Section 5, "The FEA Process" in the FEMAP User Guide
•
Section 8, "Post-Processing" in FEMAP Commands
Post Processing Overview The basic FEMAP post-processing procedure is as follows: 1. Obtain analysis results. FEMAP automatically recovers the results from many analysis programs. If your analysis program doesn’t allow this automatic recovery, you can import results (File, Import, Analysis Results). Note that analysis output data is stored in sets. If you run your model with several different loading conditions or analysis types, FEMAP will keep the output data from each analysis, mode shape, or time step in a different output set. 2. Define the type of plot and the data to be displayed. From the View Select dialog box, you can choose the type of XY, deformed, or contour plot to display. You can also select the data to be displayed. 3. Define detailed display options. From the View Options dialog box, you can control options that include the appearance of titles, deformed/undeformed model display, number of levels in a contour plot, etc.
Generating Deformation and Contour Results You can display results as deformations, contours, or combine both types of plots in the same view. From the View Select dialog box, you can select the following types of deformed and contour data: Plot Type
Description
Deformed Style: Deform
A plot of the deformed shape.
Animate
An animation of the deformed shape.
Animate MultiSet
Animation across several output sets. Good for transient, nonlinear, and frequency response analysis.
Vector
A plot showing vectors representing direction and magnitude of output.
7-2
Using Post-Processing
Plot Type
Description
Trace
Displays trace lines connecting historical positions of nodes.
Contour Style: Contour
Displays contour areas or lines.
Criteria
Displays elemental values at the centroids of elements.
Beam Diagram
Displays results along the length of line elements. Similar to 3D shear and bending moment diagrams.
IsoSurface
Displays interior surfaces of constant values in solid models.
Section Cut
Shows contours through any planar cut of a solid model.
Vector
Displays vectors at the centroids of elements.
Note: For multi-set animation and trace plots, you can also choose to animate only the contours. These types of plots can be extremely useful for heat transfer analyses.
Example A: Generating a Deformed and Contour Plot In this section of the example, you will generate a deformed and contour display.
What Open the model file containing a fan blade model and results from a linear statics analysis.
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Fanpost.MOD file.
3.
Save the model file with a different name.
Example A: Generating a Deformed and Contour Plot
7-3
What Select the deformed and contoured plot types, and specify the post-processing data for the results. Finally, you’ll specify the method used to contour the results.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Deformation: Total Translation Output Vectors: Contour: Solid VonMises Stress
5.
Contour Options
6.
Select Contour Options dialog box: Data Conversion: Max Value
7.
OK (all dialog boxes)
Notice: The data conversion options control how FEMAP converts the results from pure data at element centroids, corners, and nodes to the continuous graphical representation. In this example, you’ve chosen the maximum value using corner data. To calculate the value of an interior node in this mesh, the software takes the maximum value of the data at the corners.
7-4
Using Post-Processing
What Generate another deformed/contour plot using the averaged data conversion option.
How Step
UI
Display/Command
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Contour Options
4.
Select Contour Options dialog box: Data Conversion: Average
5.
OK (all dialog boxes)
Notice: You’ve now chosen the average value using corner data. To calculate the value of an interior node in this mesh, the software takes the average value of the data at the corners. Tip: You can use the difference in the maximum and average results to make a quick estimate of the fidelity of the model. If there is a large difference between these two contours, especially at locations that don’t have sharp corners or breaks in the model, then your model may require a finer mesh. 6.
Don’t close the model file. You will need it for Example B.
Example B: Displaying Dynamic Isosurfaces and Cutting Planes In this example, you’ll display: •
dynamic isosurfaces. You can dynamically change the value of the displayed isosurface.
•
dynamic cutting planes. You can choose an arbitrary cutting plane and dynamically pass it through a solid model.
Example B: Displaying Dynamic Isosurfaces and Cutting Planes
7-5
What Change the appearance of the plot by turning off display of the undeformed model and filled edges.
How Step
UI
1. 2. 3.
Command/Display Use the fan blade model from Example A.
F6 key
View Options View Options dialog box: Category: PostProcessing
4.
Options: Undeformed Model
5.
UNCHECK Draw Entity (turn off)
Notice: The “undeformed” model can be toggled on and off quickly using the Undeformed command from the Post Options menu on the Post Toolbar. 6.
Category: Tools and View Style
7.
Options: Filled Edges
8.
UNCHECK Draw Entity OK Notice: The “element edges” (as well as surface edges) can be toggled on and off quickly using the Filled Edges command from the View Style menu on the View Toolbar
7-6
Using Post-Processing
What View the regions of constant stress.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Display the filled edges again.
3.
View, Advanced Post, Dynamic IsoSurface Menu
4.
Dynamic IsoSurface Control dialog box: Move the slider bar. OK Notice: The display shows regions with the stress value selected on the dialog box.
What Dynamically display a plane cut.
How Step
UI
Command/Display
1.
View, Advanced Post, Dynamic Cutting Plane Menu
Generating XY Plots
Step
UI
2.
7-7
Command/Display Dynamic Section Cut Control dialog box: Move the slider bar.
Notice: The display shows contour values along a plane cut through the model. To change the plane, pick the Plane button.
3.
Save and close this model file. You will need it for Example D.
Generating XY Plots FEMAP can generate XY plots of results. The View Select dialog box also controls whether an XY plot is displayed, and the type of XY plot. The types include: Plot Type
Description
XY vs ID
Plots XY data as a function of ID number for an output vector in one output set.
XY vs Set
Plots XY data versus the output set number for an output vector across several output sets.
XY vs Set Value
Similar to XY vs Set, except that it uses the output set value for X.
XY vs Position
Plots XY data versus the position of nodes or elements along an axis direction for an output vector in one output set.
XY of Function
Plots XY data for functions. Not a post-processing option.
Example C: Generating an XY Plot In this example, you’ll display a plot of VonMises stress, then create and display a new vector of nodal stresses.
What Open the model file containing a plate model and results from a linear statics analysis.
7-8
Using Post-Processing
How Step
UI
Command/Display
1.
File, Open Menu
2.
Open dialog box: Go to the Examples directory. Open the Platepost.MOD file.
3.
Save the model file with a different name.
What Generate an XY plot of the plate top VonMises stresses.
How Step
UI
Command/Display
1.
F5 key
View, Select
2.
View Select dialog box: XY Style: XY vs Position
3.
XY Data
4.
Select XY Curve Data dialog box: Output Set: NX NASTRAN Case 1 Output Vector: 7033: Plate Top VonMises Stress OK (all dialog boxes)
Example C: Generating an XY Plot
Step
UI
7-9
Command/Display
5.
Notice: This graph plots all element centroid values vs. position, which is not very useful. You’ll create another vector below.
What Create a new vector of nodal stresses, based on the VonMises stresses.
How Step
UI
Command/Display
1.
Model, Output, Process Menu
2.
Model Output Process dialog box: Options: Convert
3.
Options: Avg
4.
Output Set: 1..NX NASTRAN Case 1
5.
Output Vector: 7033:Plate Top VonMises stress
7-10 Step
UI
Using Post-Processing
Command/Display
6.
Add Operation OK Notice: The dialog box lets you process several output operations at the same time. In this case, the software creates a new vector with nodal data that is based on the vector. The screen display won’t change.
What Make a group of the nodes on the top curve to reduce the amount of data being plotted.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Model Style: Draw Model OK
3.
Group, Set Menu
4.
Create or Activate Group dialog box: Title: Top Nodes OK
5.
Group, Node, On Curve Menu
6.
Entity Selection dialog box: Pick the straight curve on the top edge of the part. OK
Example C: Generating an XY Plot
What Plot the new group with the new nodal output vector.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: XY Style: XY vs Position
3.
XY Data
4.
Select XY Curve Data dialog box: Group: Select
5.
Group: Top Nodes
6.
Output Vector: 300000..Avg Converted Vector 7033 OK (all dialog boxes)
7.
Save the FEMAP model file. You will use it in Example E.
7-11
7-12
Using Post-Processing
Using Results Displays in Other Applications FEMAP provides several ways of using results displays in other applications. You can: •
Copy the active view to the clipboard using File, Picture, Copy. The copied data depends on which FEMAP graphics mode you are using. If you are using Render mode, a bitmap (DIB) is placed on the clipboard and if you are using non Render mode a vector image as well as a bitmap is placed on the clipboard. You can then paste the image into any other Windows program. See Example D.
•
Save the active view as a standard Windows bitmap or a Windows Device Independent Bitmap. To do this, use File, Picture, Save.
•
If the selected view is animating, create movie (AVI) files. You can also use a special bitmap format that can be displayed with the FEMAP replay program, or create a series of bitmaps to be processed by other programs to create animated GIFs for the Internet. See Example E.
•
Write the current model out as a VRML file that can be shared across the network or web with a standard VRML viewer. You can write out solid geometry or meshes.
Example D: Displaying a FEMAP Graphic in Another Application In this example, you will copy graphic displays to Microsoft Word. If you don’t have this program, try using a similar Windows application.
What Copy the deformation/contour displays to a Microsoft Word document. How Step
UI
Command/Display
1.
Open the model file that you saved at the end of Example B.
2.
Display the deformation/contour plot from Example A. Make sure that undeformed geometry is on (View Options), and that data conversion set to Average (View Select, Deformed and Contour Data, Contour Options).
3.
File, Picture, Copy Menu
Notice: This command puts a copy of the plot on the Windows clipboard.
Example D: Displaying a FEMAP Graphic in Another Application
Step 4.
UI
7-13
Command/Display Open Microsoft Word. Pick Edit, Past Special. Paste the graphic as a Device Independent Bitmap.
5.
In the Word document, enter a title for the figure.
6.
Return to FEMAP and change the data conversion option to Max Value. Generate the plot, and copy it into the Microsoft Word document. Enter another figure title.
7-14 Step
UI
7.
Using Post-Processing
Command/Display Close Microsoft Word. Close the FEMAP. You don’t need to save the model file.
Example E: Using an Animation in Another Application In this example, you will animate a deformed/contour display, save it as a movie file, and add it to a presentation created in Microsoft Power Point. (If you don’t have this program, try using a similar Windows application.)
What Animate the model.
How Step
UI
1. 2.
Command/Display Open the model file that you saved in Example C.
F5 key
View Select
3.
Model Data
4.
Select Model Data for View dialog box: Group: None Load Set: None Constraint/DOF Set: None OK
5.
Model Style: Quick Hidden Line Contour Style: Contour
6.
View Select dialog box: Deformed Style: Animate OK
Example E: Using an Animation in Another Application
Step
UI
7-15
Command/Display
Notice: The initial animation is very fast. You’ll need to adjust the speed.
What Adjust the animation speed and refine the display.
How Step
UI
Command/Display
1.
View, Advanced Post, Animation Menu
2.
Animation Control dialog box: Slower (press several times) OK
3.
Post Options (on Post Toolbar) Note: If the Post Toolbar is not showing, use the Tools, Toolbars, Post to make it visible
4.
Undeformed (toggle off)
5.
Post Options (pick the icon again) Scale Deformation
6.
Deformation Scale dialog box: 2 OK
7-16 7.
Using Post-Processing
Post Options (pick the icon) Animation Frames
8.
Animation Frames dialog box: 10 OK
9.
Post Options (icon) Animate: Positive Only (turn on)
10.
Post Options (icon) Animate Contours (turn on)
11. 12.
F6 key
View Options View Options dialog box: Category: Tools and View Style
13.
Filled Edges Draw Entity (turn off)
What Save the animation as a movie file (.AVI), and insert it into a presentation.
Example E: Using an Animation in Another Application
How Step
UI
Command/Display
1.
File, Picture, Save Menu
2.
Save Picture File As dialog box: Files of Type: Video for Windows (*.AVI) Title: Animated Plate Save OK
3.
Open Microsoft Power Point. Open an empty presentation.
4.
Insert, Movies and Sounds, Movie from File Pick the file. Double-click on the image. Notice: The image plays once.
5.
Right-click on the image. Edit Movie Object
6.
Play Object dialog box: Loop Until Stopped Rewind movie when done playing OK Notice: The image plays continuously until you end the program.
7-17
7-18 Step
7.
UI
Using Post-Processing
Command/Display
Close Microsoft Power Point. Close FEMAP. You don’t need to save the model file.
This is the end of the example. You don’t need to save the model file.
8.
Preparing Geometry for Meshing
In this example, you will learn to identify surface shapes that can cause meshing problems, then how to correct the problems to improve the mesh quality. The example includes the following steps: •
understanding the problem
•
preparing the geometry for meshing
•
creating new boundary surfaces
•
suppressing features
•
meshing the model
•
applying loads and constraints
Understanding the Problem V1
In this example, the part is a bearing block used in a large piece of industrial machinery as a simple shim. It is subject to a very large vertical load. You will be examining the amount of vertical deflection due to the vertical load. To generate a good-quality mesh on this part, you will address two issues: • Due to some fine changes in shape, the front and back faces of the part are split into three distinct faces, some of them very poorly shaped for meshing. • The part contains features (the holes) that are not important for the analysis.
ZY X To create a solid mesh, FEMAP first meshes the outside surface of the model with triangles. Every triangle is connected to three others, one on each edge. Then, based on the surface mesh, FEMAP meshes the inside volume with tetrahedral elements.
Preparing the Surfaces for Meshing
V1
If the faces of the solid are poorly shaped or degenerate, the surface mesh may have poor quality. An extremely thin face, especially one that is basically triangular, will have poor triangulation at its collapsed end. For example, here are two faces: one rectangular, one triangular When these two surfaces are meshed, the sharp triangular one will always have poor aspect ratio triangles at the sharp end.
Y ZX
V1
Y ZX Y ZX
8-2
Preparing Geometry for Meshing
As you will see in the example, in FEMAP the solution to this problem is to combine the adjacent surfaces and mesh them as one.
Suppressing Features A complex solid model may contain geometric features that are not significant enough to affect the analysis. In the example, you will suppress geometric features from the analysis without removing them from the geometric model. As a result, you can generate a much smoother mesh.
Preparing the Geometry To begin the example, you will import the geometry, then slice it in half since it is symmetrical.
Importing the Geometry What Start FEMAP and open a new model file. Import the Parasolid geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. BearingBlock.X_T Open OK
3.
View Style Menu (on View Toolbar) Choose Solid
4.
Rotate the model to an orientation similar to the following graphic.
Cutting the Geometry in Half
Step
UI
8-3
Command/Display
V1
ZY X
Cutting the Geometry in Half Since the part is symmetric, cut it in half to reduce meshing and analysis time. (Since this model is simple, you won’t save much time. However, this is an important technique for larger models.)
What Slice the symmetric part along the global ZX plane, at Y=1.
How Step
UI
Command/Display
1.
Geometry, Solid, Slice Menu
2.
Entity Selection dialog box: Double-click to select the solid.
Notice: Since there is only one solid, you can double-click to automatically select it and go to the next dialog box. 3.
Plane Locate dialog box: Methods
4.
Global Plane
5.
ZX Plane
8-4 Step
UI
Preparing Geometry for Meshing
Command/Display
6.
Y: 1 OK
V1
X 7.
ZY
Delete, Geometry, Solid Menu
8.
Entity Selection dialog box: Pick the +Y side of the solid. OK OK
V1
X
ZY
Creating New Boundary Surfaces To improve the quality of the mesh, combine some of the faces of the part to create larger boundary surfaces. The boundary surface defines an area to be meshed.
What Create boundary surfaces by combining each triangular face with the adjacent rectangular face.
Creating New Boundary Surfaces
How Step
UI
Command/Display
1.
View Style Menu (on View Toolbar) Choose Wireframe
2.
Geometry, Boundary Surface, From Surfaces on Solid Menu
3.
Entity Selection dialog box: Select one triangular face and the adjacent rectangular face. OK
4.
Select the two faces on the opposite side of the part. OK, then... Click Cancel Notice: You should now have two new boundary surfaces.
8-5
8-6
Preparing Geometry for Meshing
Suppressing Features Next, you will suppress the hole so that it will not be used in the meshing process.
What Suppress the hole.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Feature Suppression Menu
2.
Select Solid for Feature Suppression dialog box: OK Notice: Since there is only one solid, it is automatically selected.
3.
Feature Suppression dialog box: Manual
4.
Remove
5.
Loops
6.
Entity Selection dialog box: Pick a curve on the top or bottom of the hole.
Notice: When you pick loops, you pick a single curve at the top or bottom of a hole to suppress all faces underneath that loop in the topology of the solid.
Meshing the Model
Step
UI
8-7
Command/Display
7.
OK
V1
ZY X Notice: The surfaces are now gray, which means that they are suppressed. You may need to press Ctrl-G to see this change.
Meshing the Model Mesh the model using a large element size to keep the model under the 300-node demo license limit. If you have a full FEMAP installation, you might want to use a smaller element size to improve your results.
What Generate a solid mesh of the model. Set the element size to 0.5.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Define Material - ISOTROPIC dialog box: Load
3.
Select AISI 4340 Steel Click OK, then... OK again
4.
In Automesh Solids dialog box: Click Update Mesh Sizing...
8-8 Step 5.
UI
Preparing Geometry for Meshing
Command/Display In Automatic Mesh Sizing dialog box: Basic Curve Sizing: Element Size: 0.5 Click OK, then... In Automesh Solids dialog box: Click OK
V1
Z
6.
X
Y
Look in the Messages dockable pane to see information about the tet-meshing process.
Applying Loads and Constraints
Step
UI
8-9
Command/Display Notice: Your meshing diagnostic results may vary slightly from the values shown here. The key item in the diagnostics is the quality of surface triangles going into the tetrahedral mesher. Most of the triangles (98%) have aspect ratios between 1.0 and 2.0. The high quality surface mesh leads to high quality tetrahedral elements in the solid mesh.
Applying Loads and Constraints To prepare the model for analysis, apply a total vertical load to the top of the part. Fix the bottom of the part, and apply symmetric constraints.
What Apply a load of 10,000 pounds (5,000 pounds on the half symmetry model).
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set. OK 2.
Model, Load, On Surface Menu
3.
Entity Selection dialog box: Pick the top surface of the part. OK
4.
Create Loads on Surfaces dialog box: FX: 5000 OK
V1 L1
ZY X
8-10
Preparing Geometry for Meshing
What Apply a Y symmetry constraint along the symmetry cut that you made earlier. Fix the bottom of the part.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set. OK 2.
Model, Constraint, On Surface Menu
3.
Pick the surface that is the plane of symmetry. OK
4.
Create Constraints on Geometry dialog box Advanced Types: Surface
5.
Advanced Types: Sliding along Surface Click OK
6.
Pick the bottom two surfaces.
7.
Create Constraints on Geometry dialog box: Standard Types: Fixed OK
On Your Own
Step
UI
8-11
Command/Display
V1 L1 C1
ZY X
On Your Own Complete the analysis: solve the model with the NX Nastran static solver. Use the Model, Analysis command, create a new set, select “36..NX Nastran” as the Analysis Program and “1..Static” as the Analysis Type, click OK, then Analyze... button.
Once the analysis is complete, display a deformed and contour plot of T1 translation using one of the following methods: •
the View, Select command
•
the Post Data, Deformed, and Contour icons on the Post Toolbar. Also, look at the Post Options icon which contains many useful functions such as turning the “undeformed shape” on and off quickly.
•
the commands on the “context sensitive menu” of the Results branch of the Model Info tree (right click on the desired Results set to access the “context sensitive menu”).
This is the end of the example. You don’t need to save your model file.
8-12
Preparing Geometry for Meshing
9.
Repairing Sliver Geometry for Meshing In this example, you will learn to repair geometry for meshing. Slivers are small faces that are created because of numerical inaccuracies in Boolean or other solid modeling operations. Typically, these faces are much smaller than the other faces that define your solid. While they are small, they can cause great difficulties in meshing.
The example includes the following steps: •
importing the geometry with a missing sliver
•
stitching the surfaces
•
meshing the model
•
repairing problems with the geometry that caused the mesh to fail
•
meshing the new solid
Importing the Geometry What Start FEMAP and open a new model file. Import the Parasolid geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. Geometry_Repair.X_T Open OK
9-2 Step
UI
Repairing Sliver Geometry for Meshing
Command/Display
3.
View Style Menu (on View Toolbar) Choose Solid
4.
Rotate the model to an orientation similar to the following graphic.
V1
Y Z X Notice: The Parasolid file is imported as surfaces that need to be stitched together. The surfaces are assigned a random color. In this case, the sliver in the geometry is quite obvious, but often slivers are difficult to see.
Stitching the Surfaces Stitch the surfaces together to create a sheet solid, which is a type of Parasolid solid that has no volume. A sheet solid is basically a surface that you can use to perform solid surface operations, such as the Intersect, Stitch, Explode, and Slice commands.
What Stitch the surfaces back together.
How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
2.
Entity Selection dialog box: Select All OK (all dialog boxes)
Meshing the Model
Step
UI
9-3
Command/Display If FEMAP does not create a valid solid, it will temporarily turn all of the surfaces transparent, while highlighting and labeling the curves which were not stitched together.
The view will remain like this until a Window, Regenerate command has been performed using Ctrl+G or as part of another command, such as going from Solid to Wireframe using the View Style menu on the View Toolbar. Notice: The Messages dockable pane should also indicate that you’ve created a sheet solid. Tip: A sheet solid looks very similar to a regular solid. Follow the steps below to determine whether the model is a solid or a sheet solid. 3.
Tools, Mass Properties, Solid Properties Menu
4.
Select Solid for Mass Properties dialog box: Pick the solid from the list. OK No (don’t create a node and mass element), then OK for Density Notice: Examine the Messages dockable pane. If the volume has a value of 0, it is a sheet solid. If the volume has a value greater than 0, it is a regular solid. In this case, you have a sheet solid.
Meshing the Model Mesh the model containing the sliver.
What Mesh the solid model.
9-4
Repairing Sliver Geometry for Meshing
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
2.
Define Material - ISOTROPIC dialog box: Load
3.
Select From Library dialog box: Pick a material. OK (both Material dialog boxes)
4.
Automatic Mesh Sizing dialog box: OK Notice: FEMAP displays the message: “Mesher Aborted”. For more information about why the mesher failed, examine the messages in the Messages and Lists window. Tip: FEMAP first meshes the outside surface of the model. Then, based on the surface mesh, it meshes the inside volume with elements. The error message “Surface mesh has at least one hole” indicates that the tet mesher was not able to correctly mesh the surface. FEMAP aborted the meshing process and left the failed surface mesh on the model for diagnostic purposes.
5.
Tools, Undo Menu
Tip: Ctrl-Z is the shortcut for this command. Notice: Check the Messages dockable pane to make sure that you have undone the meshing command. If not, pick Undo until you have.
Repairing Problem Geometry Since meshing was aborted, you need to repair the geometry. First, try to use the geometry Cleanup command. If that doesn’t work, you’ll need to make manual repairs.
Running Cleanup
9-5
Running Cleanup The Geometry, Solid, Cleanup command checks the solid and removes any extraneous features that may have developed during export from a CAD package or from Boolean operations.
What Run the geometry Cleanup command to repair problems with the model.
How Step
UI
Command/Display
1.
Geometry, Solid, Cleanup Menu
2.
Entity Selection dialog box: Pick the solid. OK
3.
Solid Cleanup dialog box: Check the Remove Redundant Geometry, Remove Sliver Surfaces, and Check Geometry options (top three in dialog box). OK Notice: The Messages pane says that the solid has passed geometry checking. However, if you zoom and rotate the model, you will see that there is still a missing sliver.
Tip: Although the geometry passed the checker, you still may not be able to mesh it. Often, you will not be able to tell if a piece of geometry can be meshed without first trying to mesh it. With experience, you will learn what can be meshed and what needs to be modified. Before you mesh, try to visualize the size of the element and how the geometry could be constructed with it. If you can’t see how your geometry could be made from the elements, chances are the mesher won’t be able to, either.
Removing the Problem Geometry Since the geometry checker didn’t repair the geometry automatically, you will have to repair it manually. First, delete the problem surface, then create a new surface for the block.
What Explode the sheet solid into surfaces, then delete the surface that the sliver was removed from.
9-6
Repairing Sliver Geometry for Meshing
How Step
UI
Command/Display
1.
Geometry, Solid, Explode Menu
2.
Entity Selection dialog box: Pick the solid. OK
3.
Delete, Geometry, Surface Menu
4.
Entity Selection dialog box: Pick the surface that the sliver was removed from. OK, then... OK again to confirm the deletion
5.
Ctrl-G
Window, Regenerate
V1
Y Z X
Creating a New Surface Now that you have removed the problem geometry next to the sliver, you can create a new surface that can be meshed.
What When the curve was projected onto the face, the surface and the curve on one edge were split. Verify that there are two curves defining one edge.
Creating a New Surface
9-7
How Step
UI
Command/Display
1.
List, Geometry, Curve Menu
Move the cursor over the model to highlight the curves. Notice: One edge of the model will contain two curves (A and B, as shown in the figure).
A
B
What Run geometry Cleanup on the model to merge the curves. Use the new curve to create a new surface.
How Step
UI
Command/Display
1.
Geometry, Solid, Cleanup Menu
2.
Entity Selection dialog box: Select All OK
3.
Solid Cleanup dialog box: Check the Remove Redundant Geometry, Remove Sliver Surfaces, and Check Geometry options (top three in dialog box). OK
4.
Ctrl - G
5.
Window, Regenerate (the screen will verify that the curves were merged.) Geometry, Surface, Edge Curves
Menu
9-8 Step
Repairing Sliver Geometry for Meshing
UI
Command/Display
6.
Pick the four curves that made up the original surface. OK... then Cancel.
7.
Ctrl - G
Window, Regenerate
V1
Y Z X What Stitch the surfaces together.
How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
Stitch all surfaces together by clicking Select All, then... Clicking OK in all the dialog boxes Notice: Look at the Messages pane to verify that a solid was created. You can also doublecheck by using Tools, Mass Properties, Solid Properties.
Meshing the New Solid Now that you have repaired the problem geometry, you should be able to mesh it.
On Your Own
9-9
What Mesh the geometry.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids Menu
Use default values for meshing. Make sure that you load a material from the library.
On Your Own To complete the analysis: •
Apply a 100 psi pressure on the face that you corrected, and fix all of the corners.
•
Solve the model with the NX Nastran solver, using a “Linear Static” Analysis Type.
•
Display a contour of Solid von Mises Stress.
This is the end of the example. You don’t need to save your model file.
9-10
Repairing Sliver Geometry for Meshing
10.
Repairing a Mesh In this example, you will learn to repair a flawed mesh created from imported geometry.
V1
The FEMAP geometry import capability is very robust. From Parasolid systems, the capability is 100% reliable. From ACIS, IGES, STEP, Pro/ Engineer, and CATIA files, the reliability is very good. If the imported geometry contains problem surfaces, automatic meshing may not produce the best results. Sometimes it is easier to correct a bad mesh that results from bad geometry than it is to fix the bad geometry and then mesh it.
Z Y X The example includes the following steps: •
importing a flawed mesh
•
examining free edges to reveal the hole in the mesh
•
repairing the mesh problems
•
meshing the model again
Importing the Mesh What Start FEMAP and open a new model file. Import the neutral file containing the simple part with the flawed mesh.
How Step
UI
Command/Display
1.
File, Import, FEMAP Neutral Menu
2.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory. MeshFix.NEU Open OK
10-2 Step
UI
Repairing a Mesh
Command/Display
V1
Z Y X
Examining Free Edges Examine free edges to identify potential problems.
What Display free edges.
How Step
UI
Command/Display
1.
View Select (On View Toolbar)
2.
View Select dialog box: Model Style: Free Edge OK
3.
Zoom (on View Toolbar) Zoom in on the free edges.
V1
ZY X
Repairing Mesh Problems
10-3
Repairing Mesh Problems To repair the hole in the mesh, you’ll first create a group containing all the elements and free edge nodes. Next, you’ll manually create triangular mesh elements to fill the hole.
Creating a Group for Free Edge Nodes and Elements What Create a group containing the Free Edge nodes only.
How Step
UI
Command/Display
1.
Group, Set Menu
2.
Create or Activate Group dialog box: Title: Free Edge Nodes OK
3.
Group, Node, ID Menu
4.
Entity Selection dialog box: Method
5.
ID - Free Edge
6.
Entity Selection dialog box: Select the 5 nodes which are currently visible on the screen OK
What Add the elements using those “free edge” nodes to the group.
How Step 1.
UI
Command/Display View Select (On View Toolbar) or F5 key
10-4 Step
UI
Repairing a Mesh
Command/Display
2.
View Select dialog box: Model Data
3.
Select Model Data for View dialog box: Group: Active OK (All dialog boxes) Tip: For a shortcut to the Model, Data command, right-click in the graphics region. From the menu, pick Model Data.
4.
Group, Element, using Node Menu
5.
Entity Selection dialog box: Choose 1..Free Edge Nodes from the Group drop-down list.
6.
Click OK
7.
Group, Operations, Automatic Add Menu
8.
Automatically Add to Group dialog box: Active OK Notice: You have now created a group containing the free edge nodes and the elements using the free edge nodes. We are concerned with the “hole” in the mesh.
Hole in Mesh
Creating New Plate Elements
10-5
Creating New Plate Elements What Create plot planar property, then new plate elements to fill the hole.
How Step
UI
Command/Display
1.
Model, Property Menu
2.
Define Property dialog box: Click Elem/Property Type button
3.
Element/Property Type dialog box: Choose Plot Only in the Plane Elements section
4.
OK, then... In Define Property dialog box: OK, then... Yes (to question), then... Cancel
5.
Model, Element Menu
6.
Define Plate Element dialog box: Triangle
7.
Nodes: Click in the first field, then pick three nodes to create a triangular element. OK Create 2 additional elements to close the hole, then click Cancel Note: As you create elements to fill the “hole”, the free edge gets smaller.
8.
View Select (On View Toolbar)
9.
View Select dialog box: Draw Model
10-6 Step
UI
Repairing a Mesh
Command/Display
10.
Model Data
11.
Select Model Data for View dialog box: Group: None OK (all dialog boxes)
Y Z X
Meshing the Model Now that you have closed the hole using plate elements, you can generate the tetrahedral mesh. The Solids from Elements command lets you create solids from elements without the underlying geometry.
What Mesh the model with tetrahedral elements.
How Step
UI
Command/Display
1.
Mesh, Geometry, Solids from Elements Menu
2.
Entity Selection dialog box: Select All OK In Define Material - ISOTROPIC dialog box: Load
Meshing the Model
Step
UI
3.
Command/Display Select from Library dialog box: Select any material from the library
4.
OK, then... In Define Material - ISOTROPIC dialog box: OK, then... In Automesh Solids dialog box: OK
5.
Ctrl-A
Autoscale the model.
This is the end of the example. You don’t need to save your model file.
10-7
10-8
Repairing a Mesh
11.
Analyzing a Beam Model
In this example, you’ll use rod and L beam elements to represent a truss structure.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the truss
•
defining the material and property
•
meshing the model using beams and rods
•
applying constraints and loads
•
analyzing the model using NX Nastran
•
post-processing the results
Importing the Geometry What Open a new model file and import the geometry of the truss. These curves will be meshed with rod and beam elements.
How Step
UI
Command/Display
1.
File, Import, FEMAP Neutral Menu
2.
Read Model from FEMAP Neutral dialog box: Go to the Examples directory. Truss.NEU Open OK
11-2 Step
UI
Analyzing a Beam Model
Command/Display
Y
X Z
Defining the Material and Property The first step for the meshing process will be to define the material and property for the beam and rod elements.
Defining the Material What Define the material by selecting a standard material from the FEMAP material library.
How Step
UI
Command/Display
1.
Model, Material Menu
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). 2.
Define Material - ISOTROPIC dialog box: Load
3.
Select from Library dialog box: AISI 4340 Steel OK OK, then... Cancel
Defining the Beam Property FEMAP has a library of general cross sections for you to choose from, but you may not always want to use them. You can define an arbitrary cross section by creating a surface in FEMAP, or by importing external geometry. FEMAP will then calculate the section properties from that surface.
Defining the Beam Property
11-3
The neutral file that you imported has a boundary surface on a different layer that is not currently shown. You will now display it.
What First, hide the default layer. Next, display the boundary surface on a hidden layer.
How Step
UI
Command/Display
1.
View, Layers Menu
Tip: You can also pick the Layers icon
on the View Toolbar to open this dialog box.
You can also use the Manage command from the “context sensitive menu” located on the Layers branch in the Model Info tree (simply click to highlight any Layer, then right mouse click to see the context sensitive menu). 2.
Layer Management dialog box: Visible Layers: Default Layer
3.
Click Hide
4.
Hidden Layers: Beam Section
5.
Click Show OK
6.
Ctrl - A
Autoscale Notice: The boundary section and curves are displayed.
Y
X Z
11-4
Analyzing a Beam Model
What Define a property for the beam elements. You’ll first create a general beam cross section, then define a vector to define the section’s Y axis. Next, you’ll define the beam property with the cross section and the AISI 4340 material that you’ve created.
How Step
UI
Command/Display
1.
Model, Property Menu
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). 2.
Define Property dialog box: Elem/Prop Type
3.
Element Property Type dialog box: Line Elements: Beam OK
4.
Define Property dialog box: Shape
5.
Cross Section Definition dialog box: Shape: General Section
6.
Surface
7.
Select Surface to Check dialog box: Click on the surface. OK
8.
Vector Locate - Define Section Y Axis dialog box: Base: 0, 0, 0 (make sure these are the X,Y,Z values for the base) Tip: 0, 1, 0 (enter these X,Y,Z values for the tip) OK Notice: This vector defines the Y axis for the section.
9.
Cross Section Definition dialog box: OK
Meshing the Model
Step
UI
10.
11-5
Command/Display Define Property dialog box: Title: General Beam Section Notice: The calculated section properties are now displayed in this dialog box.
11.
Material: AISI 4340 Steel OK, then... Cancel
Meshing the Model This model will be meshed with two types of elements: beam elements on the longitudinal curves, and rod elements on the curves that connect the beams. Once you’ve created the elements, you’ll merge the coincident nodes.
Creating the Beam Mesh First, mesh the longitudinal curves with beams whose properties were defined in the previous section.
What Hide the beam section and show the default layer.
How Step
UI
1.
Command/Display Layers (on View Toolbar)
Tip: You can also “Hide and Show” layers directly from the Layers branch in the Model Info tree. Simply pick on any number of layers (hold down the Ctrl or Shift key to select Multiple layers), then choose the Hide or Show command from the “context sensitive menu”. 2.
Layer Management dialog box: Hide the Beam Section, and show the Default Layer. OK
3.
Ctrl - A
Autoscale
11-6 Step
UI
Analyzing a Beam Model
Command/Display V1
Y
X Z
What Rotate the model to get a trimetric view for meshing.
How Step
UI
Command/Display
1.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 2.
View Rotate dialog box: Trimetric OK
What Mesh the longitudinal curves with beams. You’ll use the general beam cross section to define the beam. After you select the cross section, you’ll enter a vector to define the beam element orientation. It’s important that this vector be identical to the one used to define the cross section properties; otherwise, your analysis results may be incorrect.
How Step
UI
Command/Display
1.
Mesh, Geometry, Curve Menu
2.
Entity Selection dialog box: Pick the curves highlighted in the following figure. OK
Creating the Beam Mesh
Step
UI
3.
Command/Display
Geometry Mesh Options dialog box: Property: General Beam Section OK
4.
Vector Locate dialog box: Base: 0, 0, 0 (make sure these are the X, Y, Z values for the base) Tip: 0, 1, 0 (enter these X, Y, Z values for the tip) OK V1
Y X Z
What Display the beam elements with their cross sections visible.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Element Orientation/Shape (select) Element Shape: Show Cross Section (select) OK
11-7
11-8 Step
UI
Analyzing a Beam Model
Command/Display
Tip: You can also “toggle” the cross-sections of line elements on/off using the “Thickness/ Cross Section” command from the View Style menu located on the View Toolbar.
What Rotate and zoom the model to get a better look at the cross section. Your cross section may have an incorrect orientation that you need to modify.
How Step
UI
Command/Display
1.
Rotate the model slightly to the see the cross sections better.
2.
Zoom (on View Toolbar)
Notice: Compare your beams with the following diagram. Note that the “notch” on each cross section faces the inside of the part. If some of your beams are oriented differently, you will need to modify them. The following steps show you how to reverse the normals when they are facing in the wrong direction. It is normal for you to need to modify the normal direction of some of your beams to make it look like the figure below.
Creating the Rod Mesh
Step
UI
11-9
Command/Display
3.
Modify, Update Elements, Line Element Reverse Direction Menu
4.
Entity Selection dialog box: Pick the elements to modify. (Pick only the elements with cross sections facing in the wrong direction.) OK
5.
Ctrl - A
Autoscale
Creating the Rod Mesh You will now mesh the remaining curves with rod elements to connect the beams.
What Mesh the curves. You’ll also need to create a new property to define the rods.
11-10
Analyzing a Beam Model
How Step
UI
Command/Display
1.
Mesh, Geometry, Curve Menu
2.
Entity Selection dialog box: Pick all of the unmeshed curves: the cross braces and the connection between the two rows of beams. OK
3.
Geometry Mesh Options dialog box: New Prop Notice: You only have the General Beam Section property in your model. You’ll need to create a rod property.
4.
Define Property dialog box: Elem/Property Type
5.
Line Elements: Rod OK
6.
Define Property dialog box: Title: 2 in Diam Rod
7.
Area: 3.14
8.
Material: AISI 4340 Steel OK
9.
Geometry Mesh Options dialog box: OK Notice: The property you created is selected for the element’s property. Notice: The curves are meshed with rod elements.
Merging Coincident Nodes
Step
UI
11-11
Command/Display
What Reduce the amount of information displayed by turning off the display of geometry and labels.
How Step
UI
Command/Display
1.
Ctrl - Q
View Quick Options dialog box:
Notice: You can also turn on this dialog box with the Quick Options toolbar icon 2.
Geometry Off Labels Off Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry and Labels on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. The third icon allows you to toggle Labels on and off.
Merging Coincident Nodes Because the curves were meshed with two meshing operations, there will be nodes at the ends of both the beam and rod elements. You will merge these coincident nodes to effectively “sew” the model together.
What Merge the coincident nodes.
11-12
Analyzing a Beam Model
How Step
UI
Command/Display
1.
Tools, Check, Coincident Nodes Menu
2.
Entity Selection dialog box: Select All OK
3.
Check/Merge Coincident dialog box: Options: Merge Coincident Entities (check) OK Notice: Look in the Messages dockable pane to see how many coincident nodes have been merged. All rod and beam elements are now connected together.
Applying Constraints and Loads You will create a constraint set to model symmetry and fix the end. The symmetry of the truss will be used to reduce the model to half the size. You will also apply a load to this model to simulate something hanging from the truss.
Modeling Symmetry and a Fixed End To simulate the symmetry of this part, you will constrain the four nodes that are at the halfway point of the structure. You are defining symmetry across the X-plane through these four points. By imposing this type of constraint condition, you are actually introducing a stiffness exactly equal to the structure modeled, just mirrored above the X-plane.
What Create the constraints to model symmetry and fix the end. You’ll also constrain the rest of the model in all DOF except the X and Y translations.
How Step
UI
Command/Display
1.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 2.
View Rotate dialog box: Isometric OK
Modeling Symmetry and a Fixed End
Step
UI
11-13
Command/Display
3.
Model, Constraint, Nodal Menu
Notice: First, you’ll apply constraints at these nodes to model symmetry. 4.
Create or Activate Constraint Set dialog box: Title: (enter a title) OK
5.
Entity Selection dialog box: Pick nodes A, B, C, and D (see the following figure). OK
A D B C 6.
Create Nodal Constraints/DOF dialog box: X Symmetry OK Notice: The TX, RY, and RZ DOF are selected. Because you are applying nodal constraints, you could control the constraint of each degree of freedom individually in the dialog box, or you can use the quick keys to apply common constraint conditions.
7.
Entity Selection dialog box: Pick nodes E and F (see the following figure). OK Notice: You are now fixing the nodes on the opposite end.
11-14 Step
UI
Analyzing a Beam Model
Command/Display F E
8.
Create Nodal Constraints/DOF dialog box: Fixed OK Notice: All DOF are selected.
9.
Entity Selection dialog box: Select All OK Notice: Finally, you’ll restrain the DOF for all nodes in the Z translation and all rotations.
10.
Create Nodal Constraints dialog box: DOF: TZ, RX, RY, RZ (check) OK
11.
No (to combine the constraints)
What Turn off element cross sections to better see the constraints.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Element Orientation/Shape (select) Element Shape: Line/Plane Only (select) OK
Applying a Load to the Model
Step
UI
11-15
Command/Display
Tip: If you turn the constraint labels back on, you’ll see the degree of freedom numbers displayed for each constraint. (To do this, pick F6. Pick Options, Constraint. Under Label Mode, pick Degree of Freedom.)
Applying a Load to the Model You will now apply a load in the negative Y direction to simulate something hanging from this truss. Like constraints, loads are grouped in sets. Before creating any loads, you must create a set to hold them.
What Create the load in the negative Y direction.
How Step
UI
Command/Display
1.
Model, Load, Nodal Menu
2.
Create or Activate Load Set dialog box: Title: (enter a title) OK
3.
Entity Selection dialog box: Pick nodes A and B. OK
11-16 Step
UI
Analyzing a Beam Model
Command/Display
B A
4.
Create Loads on Nodes dialog box: FY: Value: -200 OK Notice: The default load type is force.
Analyzing the Model Analyze the model using the NX Nastran solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: New
Post-Processing the Results
Step
UI
11-17
Command/Display
3.
Analysis Set dialog box: Title: (enter a title for the solve)
4.
Analysis Program: 36..NX Nastran Analysis Type: 1..Static OK
5.
Analyze
Post-Processing the Results For this example, you will display two types of results: criteria plots and beam diagrams.
Displaying Criteria Diagrams As an alternative to contours, you can use a basic criteria display that shows the output value of each element. The primary purpose of a criteria display, however, is to limit the display based on a selected criteria.
What Display a basic criteria view of the results.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform
3.
Contour Style: Criteria
4.
Deformed and Contour Data
5.
Select PostProcessing Data dialog box: Output Vectors: Deformation: Total Translation Contour: 3022..Beam EndA Axial Force OK (all dialog boxes)
6.
View, Rotate, Model Menu
11-18 Step
UI
Analyzing a Beam Model
Command/Display Tip: You can press the F8 key instead of using the command above.
7.
View Rotate dialog box: Trimetric OK
What To reduce clutter, turn off display of undeformed elements.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Category: PostProcessing
3.
Options: Undeformed Model
4.
UNCHECK Draw Entity OK
Displaying Criteria Diagrams
Step
UI
11-19
Command/Display
What Modify the criteria for the elements to be displayed. Display the elements above the maximum limit of 350.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Notice: The PostProcessing category is already selected.
3.
Options: Criteria Limits
4.
Minimum: 0 Maximum: 350
5.
Limits Mode: Above Maximum OK
Notice: Only the elements with axial force values above 350 are displayed as shaded beams; the other elements don’t have color.
11-20 Step
UI
Analyzing a Beam Model
Command/Display
Displaying Beam Diagrams To conclude the example, you’ll generate beam diagrams of the axial stress. Beam diagrams display results along the length of line elements. You can set options to control the direction of beam diagrams.
What Generate a beam diagram of beam end axial stress.
How Step
UI
Command/Display
1.
View Select (On View Toolbar)
2.
View Select dialog box: Deformed Style: None - Model Only Contour Style: Beam Diagram
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Contour: 3139..Beam EndA Pt1 Comb Stress OK (all dialog boxes)
Displaying Beam Diagrams
Step
UI
11-21
Command/Display
What You can change the plane where the beam diagram will be drawn. FEMAP always draws the diagram in the plane that you choose, even if the output is actually based on forces/stresses in a different plane.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Options: Beam Diagram Default Direction: Element Z OK Notice: The beam diagrams are now drawn on the element Z plane.
11-22 Step
UI
Analyzing a Beam Model
Command/Display
This is the end of this example. You don’t need to save the model file.
12.
Analyzing an Axisymmetric Model In this example, you will take advantage of the axisymmetric nature of a pressure vessel and analyze the part using axisymmetric elements. The example includes the following steps: • importing the geometry • meshing the model • applying constraints and loads • analyzing the model using NX Nastran • post-processing the results
Importing the Geometry To begin the example, you will import the geometry of a pressure vessel that was created in AutoCAD. The geometry was exported from AutoCAD as an AutoCAD DXF file. DXF files are popular for transferring geometry between CAD programs and desktop publishing software.
What Start FEMAP and open a new model file. Import the geometry file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
2.
Geometry File to Import dialog box: Go to the Examples directory. Vessel.DXF Open OK
12-2 Step
Analyzing an Axisymmetric Model
UI
Command/Display
V1
Y ZX
Meshing the Model You will first set the global mesh size, then define the materials and properties for the mesh. Next, you will create a boundary surface and mesh the part.
Setting the Global Mesh Size As the first step in the meshing process, you will set the global mesh size then view it to verify that mesh spacing is appropriate.
What Set the global mesh size.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Default Size Menu
2.
Default Mesh Size dialog box: Size: 0.25 OK
3. 4.
F6 key
View Options View Options dialog box: Curve - Mesh Size Show As: 2..Symbols (all curves) OK
Creating the Material and Property
Step
UI
12-3
Command/Display Notice: You should see small dots/diamonds along each of the geometric entities in FEMAP. These dots/diamonds indicate where nodes will be created during any automatic meshing commands that use this geometry.
V1
Y Z X
Creating the Material and Property Create the material and property for the elements.
What Create the material by selecting a standard material from the FEMAP material library.
How Step
UI
Command/Display
1.
Model, Material Menu
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). 2.
Define Material - ISOTROPIC dialog box: Load
3.
Select from Library dialog box: 15-5PH Stainless H1025 (select) OK OK, then... Cancel
12-4
Analyzing an Axisymmetric Model
What Create the property for the axisymmetric mesh elements.
How Step
UI
Command/Display
1.
Model, Property Menu
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). 2.
Elem/Property Type
3.
Element Property Type dialog box: Volume Elements: Axisymmetric OK
4.
OK to show Axisymmetric Axis in all Views: Yes
5.
Define Property dialog box: Title: Axisymm 15-5PH
6.
Material: 15-5PH Stainless H1025 OK, then... Cancel
What Correct the axisymmetric axis orientation. This axis gives a visual cue to the orientation of the model and for axisymmetric shell elements, provides the axis used to define load direction.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Category: Tools and View Style
Meshing the Model
Step
UI
12-5
Command/Display
3.
Options: Axisymmetric Axes
4.
Direction: Global Y, X Radial OK
Meshing the Model This shape could be broken down into simple geometric regions for mapped meshing, but it is much easier to create a FEMAP boundary surface and automatically mesh the whole part.
What Create a boundary surface.
How Step
UI
Command/Display
1.
Geometry, Boundary Surface, From Curves Menu
2.
Entity Selection dialog box: Select All OK, then... Cancel
V1
Y ZX What Generate a mesh of the model.
12-6
Analyzing an Axisymmetric Model
How Step
UI
Command/Display
1.
Mesh, Geometry, Surface Menu
2.
Entity Selection dialog box: Pick the boundary. OK
3.
Automesh Surfaces dialog box: Property: Axisymm 15-5PH Stainless H1025
4.
Element Shape: All Triangles
5.
Fast Tri-Mesh (turn on - if not on by default) OK
6. 7.
Ctrl-Q
View Quick Options View Quick Options dialog box: Geometry Off Labels Off Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry and Labels on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. The third icon allows you to toggle Labels on and off.
Applying Constraints and Loads
Step
UI
12-7
Command/Display
V1
Y ZX
Applying Constraints and Loads To prepare the model for analysis, constrain the base of the model, and apply a pressure load. Since this model is axisymmetric, there is no need to apply any constraints on loads out of plane.
Defining Constraints What Constrain the bottom nodes along the flat edge against vertical movement.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set. OK 2.
Model, Constraint, Nodal Menu
3.
Entity Selection dialog box: Pick the four nodes along the bottom of the part (see following figure). OK
12-8 Step
Analyzing an Axisymmetric Model
UI
Command/Display
V1 L1 C1
Y Z X 4.
Create Nodal Constraints/DOF dialog box: TY OK
V1 L1 C1
Y ZX
Defining Loads In an axisymmetric model, a pressure load is applied to the edges of the axisymmetric elements. Since the load is applied to the edges of the elements, FEMAP requires you to specify the element and which face of the element gets the load. Here you will use the Adjacent Faces method to apply loads to the model.
What Apply a pressure load to the interior faces of the elements.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set. OK 2.
Model, Load, Elemental Menu
Defining Loads
Step 3.
UI
12-9
Command/Display Entity Selection dialog box: Select All OK
4.
Create Loads on Elements dialog box: Pressure: Value: 100 OK Tip: In this example, you are applying a pressure load to edges. However, if you wanted instead to apply a nodal force load to an axisymmetric model, some solvers require that you define the load data as force/length/radian, while others use force/length/degree. Be sure to check your analysis software’s documentation to verify which convention is appropriate.
5.
Face Selection for Elemental Loads dialog box: Method: Adjacent Faces
6.
Face (click in field) Notice: Clicking in this field moves the focus (the flashing cursor) there. When you select from the Graphics window, FEMAP will know that you are trying to pick a face.
7.
Pick an element face on the inside of the part.
V1 L1 C1
Y ZX 8.
Tolerance: 85 OK Notice: The Adjacent Faces method selects connected free faces (edges, in this case) until it finds a connected free face that exceeds the angle tolerance. In this example, by entering a very large angle tolerance of 85 degrees, the software selects all the internal faces up to the corners along the Y axis. To go around this corner, you would need to enter an angle of 90 degrees or greater.
12-10 Step
UI
Analyzing an Axisymmetric Model
Command/Display
Analyzing the Model Solve the model using the NX NASTRAN solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Create an analysis set.
2
Select the “36..NX Nastran” from the Analysis Program drop down menu Select “1..Static” from the Analysis Type drop down menu. Use all default values.
3.
Analyze
4.
Yes (verify that it’s OK to flip the model) Yes again (force all element normals to lie along the correct global axis)
Post-processing the Results
Step
UI
12-11
Command/Display Tip: NX Nastran also makes the following assumptions for an axisymmetric model:
5.
•
The Z axis is the axis of symmetry.
•
The X axis is in the radial direction.
•
All nodes must lie in the X-Z plane of the global coordinate system, and must have a nonnegative X (radial) coordinate.
•
All loads must be in the X-Z plane.
•
The Y axis of all nodal displacement coordinate systems must be parallel to the global Y axis.
•
XY and YZ shear stresses and strains are zero.
•
All gravity vectors must be parallel to the axis of symmetry.
•
All angular velocity vectors must lie on the axis of symmetry.
Scale Factor for Axisym Forces dialog box: OK Tip: The scale factor does not affect the pressures that you defined for this example. However, if you define nodal forces for an axisymmetric model, the scale factor lets you convert nodal load values for use with a different solver. For instance, suppose that you have defined a nodal force value for a solver that uses units of force/length/degree. To analyze the model with a different solver, you can use the scale factor to convert the nodal load value to units of force/length/radian.
6.
Yes (To permanently convert the elements to triangular elements with midside nodes) Yes again (to save the model so you can view the results in the correct model)
Post-processing the Results For this analysis, you will display deformation and stress contours.
What Display and deformed/contour plot of translation and Azimuth (hoop) stress for the pressure vessel part.
How Step
UI
Command/Display
1.
F8 key
View Rotate Model
2.
View Rotate dialog box: ZX Front OK
12-12 Step
UI
Analyzing an Axisymmetric Model
Command/Display
V1 L1 C1
Z Y X 3.
F5 key
4.
View Select View Select dialog box: Deformed Style: Deform Contour Style: Contour
5.
Deformed and Contour Data
6.
Select PostProcessing Data dialog box: Output Vectors: Deformation: 1. Total Translation Output Vectors: Contour: 6029: Axisym Azimuth Stress OK (all dialog boxes)
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
8.
In View Quick Options dialog box:
UNCHECK Node box located in the Geometry section, then
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Nodes on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
Post-processing the Results
Step
UI
Command/Display
9.
F6 key
View Options
10.
View Options dialog box: Category: PostPorcessing
11.
Options: Undeformed Model
12.
Draw Entity: OK
This is the end of the example. You don’t need to save your model file.
12-13
12-14
Analyzing an Axisymmetric Model
13.
Analyzing a Midsurface Model of a Welded Pipe
In this example, you will model a welded pipe to determine the force distribution along the weld line between the two tubes. L O A D
Fixed
Fixed
To use this model with the 300-node demonstration version, you will model a midsurface shell mesh on a quarter of this part, then use symmetrical boundary conditions to represent the remaining three-quarters of this model. The example includes the following steps: •
importing the geometry using the Parasolid interface
•
slicing the model
•
creating the midsurface model
•
meshing the model
•
applying loads and constraints
•
analyzing the model using NX Nastran
•
post-processing the grid-point force balance results using Freebody Display
Importing the Geometry To begin the example, you will import the geometry.
What Start FEMAP and open a new model file. Import the Parasolid geometry file.
13-2
Analyzing a Midsurface Model of a Welded Pipe
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the Examples directory. Import the Pipe.X_T file. 2.
Solid Model Read Options dialog box: OK
3.
Rotate the model to the orientation shown.
V1
Y X Z
Slicing the Model Slice the model so that the -X quarter remains.
What Slice through the XY global axis at Z=5.0. Next, slice the model through the global YZ axis at X=0.0.
How Step
UI
Command/Display
1.
Geometry, Solid, Slice Menu
2.
Entity Selection dialog box: Pick the solid. OK
Slicing the Model
Step
UI
Command/Display
3.
Plane Locate dialog box: Methods
4.
Global Plane
5.
XY Plane
6.
Z: 5.0 OK
7.
Geometry, Solid, Slice Menu
Select the +Z solid (Solid on right in view below). Slice the solid along the YZ global plane at X = 0.0.
V1
Y X Z What Delete the -Z half and +X quarter of the model.
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
13-3
13-4 Step
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
2.
Entity Selection dialog box: Pick the -Z half of the model. (Solid on left in above figure) OK OK
3.
Delete, Geometry, Solid Menu
Delete the +X half of the model.
V1
Y X Z
Creating the Midsurface Model Create the midsurface model, then delete the original solid. Stitch the unconnected surfaces together to form one piece of geometry.
Creating the Midsurface What Use the automatic midsurfacing capability to create a midsurface model.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Automatic Menu
2.
Entity Selection dialog box: Select All OK
Creating the Midsurface
Step
UI
3.
13-5
Command/Display Midsurface Tolerance dialog box: Move the cursor to the Graphics window.
4.
Ctrl-D Notice: The Ctrl-D command lets you determine distance for the target thickness. The software uses this value to determine which surfaces to place a midsurface between. The target thickness should be slightly larger than the largest distance between the planes on the solids that you want midsurfaced. If the target thickness is too low, the midsurfaces will not be created. If the target thickness is too high, some midsurfaces will be created between the wrong surfaces.
5.
Locate dialog box: Methods
6.
On Point
7.
Move the cursor to the Graphics window. Snap to Point
8.
On Point dialog box: Pick point A (see following figure). OK Note: If you have trouble picking, click in the Point ID field to reset the picking focus.
V1
A B
X YZ 9.
Pick point B. OK
13-6 Step
Analyzing a Midsurface Model of a Welded Pipe
UI
Command/Display
10.
Midsurface Tolerance dialog box: OK (accept the value calculated by the Ctrl-D command) Notice: The target thickness value should be approximately 0.1.
Tip: The Geometry, Midsurface, Automatic command is actually a combination of three commands: (1) Geometry, Midsurface, Generate; (2) Geometry, Midsurface, Intersect; and (3) Geometry, Midsurface, Cleanup. If the Automatic command has removed necessary midsurfaces, you can work through the midsurfacing commands one at a time, so that you can more easily pick which surfaces should be kept.
Deleting the Solid What Delete the original solid.
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
2.
Entity Selection dialog box: Pick the solid. OK OK
Stitching the Geometry
Step
UI
13-7
Command/Display
V1
Y XZ
Stitching the Geometry Connect the three surfaces together into one piece of geometry.
What Stitch the three surfaces together. How Step
UI
Command/Display
1.
Geometry, Solid, Stitch Menu
2.
Entity Selection dialog box: Select All OK
3.
Surface/Solid Stitching dialog box: OK You will notice that the model will become transparent and the curves which were not stitched together will be highlighted and labeled. This lets you know all of the internal surfaces are now part of the same sheet solid.
13-8
Analyzing a Midsurface Model of a Welded Pipe
Meshing the Model The first step in meshing the model is to assign mesh attributes for the different surfaces. If the correct attributes are not assigned, the results won’t be accurate. Next, set the size for the mesh. Finally, mesh the midsurface.
Assigning Mesh Attributes What Assign the mesh attributes to the surfaces.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Assign Mesh Attributes Menu
2.
Entity Selection dialog box: Select All OK
3.
Define Material - ISOTROPIC dialog box: Load
4.
AISI 4340 Steel OK (all dialog boxes)
Notice: Each surface now has a material property assigned to it.
Meshing the Model What Set the mesh size to the default value, and mesh the model.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
Meshing the Model
Step
UI
13-9
Command/Display
2.
Entity Selection dialog box: Select All OK
3.
Automatic Mesh Sizing dialog box: Element Size: 0.3 OK Note: FEMAP will display small diamonds that indicate the mesh seed locations along the edges of the surfaces being meshed.
4.
Mesh, Geometry, Surface Menu
5.
Entity Selection dialog box: Select All OK
6.
Automesh Surfaces dialog box: OK Note: The Property field is filled in with “Use Meshing Attributes”.
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
13-10 Step
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
8.
In View Quick Options dialog box:
UNCHECK Surface box located in the Geometry section, then
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Surfaces on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
Applying Loads and Constraints You will apply a load that represents 1000 pounds vertical. Since the model is symmetric, you’ll also need to apply constraints to define this symmetry. What Apply a load that represents 1000 pounds vertical (+Y). Since you have modeled only one-quarter of the part, you need to apply a load of 250 to the top curve.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Applying Loads and Constraints
Step
UI
Command/Display
2.
Create or Activate Load Set dialog box: Title: (enter a title) OK
3.
Model, Load, On Curve Menu
4.
Entity Selection dialog box: Pick the top curve as shown in the following figure. OK
5.
Create Loads on Curves dialog box: FY: 250 OK
13-11
13-12
Analyzing a Midsurface Model of a Welded Pipe
What Apply nodal constraints to the symmetric edges, and fix one edge of the part.
X Symmetry
Z Symmetry
Z Symmetry Fixed
X Symmetry
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Model, Constraint, Nodal Menu
3.
Entity Selection dialog box: Method
4.
On Curve
5.
Pick the two curves shown below. OK
Applying Loads and Constraints
Step
6.
UI
Command/Display
Create Nodal Constraints/DOF dialog box: Z Symmetry OK
7.
Entity Selection dialog box: Pick the three curves shown in the following figure. OK
8.
Create Nodal Constraints/DOF dialog box: X Symmetry OK No (to combine, not overwrite)
9.
Entity Selection dialog box: Pick the curve shown in the following figure. OK
13-13
13-14 Step
UI
10.
Analyzing a Midsurface Model of a Welded Pipe
Command/Display
Create Nodal Constraints/DOF dialog box: Fixed OK No (to combine, not overwrite)
11. 12.
Crtl-Q
This will bring up View Quick Options dialog box: In View Quick Options dialog box: Labels Off Click Done
Analyzing the Model Solve the model using the NX Nastran solver.
What Create the analysis set and solve the model.
Post-processing the Results
13-15
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: Create a new analysis set. Select the “36..NX Nastran” from the Analysis Program drop down menu Select “1..Static” from the Analysis Type drop down menu. OK
3.
Master Requests and Conditions (double-click to expand) Output Requests (select)
4.
Edit
5.
Output Requests dialog box: Nodal: Force Balance (check)
6.
In the Customization portion of the dialog box select: Results Destination: 2..PostProcess Only Notice: Using “2..PostProcess Only” will force NX Nastran to create output in a binary file (.op2 file) instead of in the print file (.f06 file). The .f06 file does not contain the Grid Point Force data required for FEMAP to create a Freebody Diagram. Also, “3..Print and Post” can not be used to retrieve Grid Point Force data. This is because FEMAP always reads in the .f06 file first to attain any error, warning, and information messages. If the .f06 contains output, FEMAP will read that output in and skip the read of the .op2 file. Tip: When you pick the force balance option, NX Nastran will output all the forces that act on each node of the model from all elements connected to that node. With this information, you can create a freebody diagram of the model or any portion of the model.
7.
Click OK, then... Click Analyze
Post-processing the Results For this analysis, you will generate a freebody display. You will first group the elements in the model to split it along the weld line. You can then view a freebody diagram of part of the model, thus displaying forces along the weld.
What Create a group of the nodes and elements of the lower surface.
13-16
Analyzing a Midsurface Model of a Welded Pipe
How Step
UI
Command/Display
1.
Group, Set Menu
2.
Create or Activate Group dialog box: ID: 2 Title: Lower Surface OK Notice: Group 1 was automatically created when you generated midsurfaces.
3.
Group, Element, On Surface Menu
4.
Entity Selection dialog box: Pick the lower surface. OK
5.
Group, Node, On Surface Menu
6.
Entity Selection dialog box: Pick the lower surface. OK
7.
Grp (click on the Status bar at the bottom of the FEMAP window)
Post-processing the Results
Step
UI
8.
13-17
Command/Display Pick Group 2 to make it active.
Notice: The Status bar lists the active group (for example, Grp:2). 9.
Grp (Status bar)
10.
View Active
Tip: You can also manage groups using the Model Info tree. Double click on any group to make it the “Active” group and you can toggle on and off the View Active command using the “context-sensitive menu” available by right-clicking on any Group. There many other functions which can be performed with the “context-sensitve menu” for Groups.
What Generate a freebody display.
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Select PostProcessing Data dialog box: Freebody Display
4.
View Freebody Options dialog box: Freebody Style: Show Freebody Display (check)
5.
Freebody Group: Active (turn on)
13-18 Step 6.
UI
Analyzing a Midsurface Model of a Welded Pipe
Command/Display Freebody Options: Show Forces (check) Show Moments (turn off) Entity Colors (check) Show Load Summation (check) Show Freebody on All Internal Nodes (turn off) Scale Vectors by Magnitude (turn off) Minimum Vector Magnitude (check) Display Vector Components (check) Y (check) X and Z (turn off) OK (all dialog boxes)
Notice: Since you are only viewing Y components of force, you see the vertical reaction forces at the fixed end of the part as well as the vertical load transfer through the nodes at the welded interface. Note the variation in vertical load transfer through the welded connection. Calculating an effective length for a node with the highest force (99.852 pounds) indicates a running load of approximately 359.5 pounds/inch. If you were to assume an equal distribution of load along the joint, the running load would have been 17.7 pounds per inch. This is the end of the example. You don’t need to save your model file.
14.
Analyzing a Midsurface Model of an Electrical Box In this example, you will learn to work with FEMAP’s semi-automatic midsurface extraction capabilities to build an idealized model of an electrical box. To work through this example, you must have a licensed copy of NX Nastran for FEMAP. You will not be able to complete this example with the 300-node demo version.
The example includes the following steps: •
importing the geometry using the STEP interface
•
creating the midsurface model
•
meshing the model
•
applying loads and constraints
•
analyzing the model using NX Nastran
•
post-processing the results
Importing the Geometry To begin the example, you will import the geometry.
What Start FEMAP and open a new model file. Import the STEP file.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the Examples directory. Import the mp.STP file. 2.
STEP Read Options dialog box: OK
14-2 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
3.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 4.
View Rotate dialog box: Dimetric OK
5.
View Style Menu (on View Toolbar) Choose Wireframe
Creating the Midsurface Model Create the midsurface model, then delete the original solid. Once the midsurface has been generated, you will need to so some additional cleanup work on the geometry before you can mesh it.
Creating the Midsurface What Use the automatic midsurfacing capability to create a midsurface model.
How Step 1.
UI
Command/Display Zoom and rotate the part to get a better view of the points we will be picking to designate the “Target Distance” for midsurfacing.
Creating the Midsurface
Step
UI
14-3
Command/Display
2.
Geometry, Midsurface, Automatic Menu
3.
Entity Selection dialog box: Select All OK
4.
Midsurface Tolerance dialog box: Move the cursor to the Graphics window.
5.
Ctrl-D Notice: The Ctrl-D command lets you determine distance for the target thickness. The software uses this value to determine which surfaces to place a midsurface between. The target thickness should be slightly larger than the largest distance between the planes on the solids that you want midsurfaced. If the target thickness is too low, the midsurfaces will not be created. If the target thickness is too high, some midsurfaces will be created between the wrong surfaces.
6.
Locate dialog box: Methods
7.
On Point
8.
On Point dialog box: Pick point A (see following figure). OK
14-4 Step
Analyzing a Midsurface Model of an Electrical Box
UI
Command/Display
V1
A B
ZY X 9.
Pick point B. OK
10.
Midsurface Tolerance dialog box: OK (accept the value calculated by the Ctrl-D command) Notice: The target thickness value should be approximately 4.9.
V1
Z Y X
Deleting the Solid What Delete the original solid.
Cleaning Up the Geometry
How Step
UI
Command/Display
1.
Delete, Geometry, Solid Menu
2.
Entity Selection dialog box: ID: 1 OK OK
3.
View Style Menu (on View Toolbar) Choose Solid
Cleaning Up the Geometry To create a more accurate midsurface model, you must trim each rib, then delete the top portion.
What Trim the surface of each rib.
14-5
14-6
Analyzing a Midsurface Model of an Electrical Box
How Step
UI
Command/Display
1.
Geometry, Midsurface, Trim with Curve Menu
2.
Select Surface/Solid to Trim dialog box: Pick one of the eight ribs. OK
C
3.
Entity Selection dialog box: Pick the curve on the lower portion (see C above). OK Notice: The curve now cuts through the surface.
V1
Z Y X 4.
Repeat the process to trim the other seven ribs.
Cleaning Up the Geometry
Step
UI
14-7
Command/Display Tip: When you are performing any command in Render mode (Default graphics mode), you can hold down the middle mouse button to rotate the model.
What Delete the top portion of each rib. How Step
UI
Command/Display
1.
Delete, Geometry, Surface Menu
2.
Entity Selection dialog box: Pick the new surfaces that have been created on the top of each rib (see D in the following figure). OK OK
D
Notice: The top of each rib has been deleted.
14-8
Analyzing a Midsurface Model of an Electrical Box
What .Intersect the new ribs with the walls of the electric box.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Intersect Menu
2.
Entity Selection dialog box: Select All OK
Meshing the Model The first step in meshing the model is to assign mesh attributes for the different surfaces. If the correct attributes are not assigned, the results won’t be correct. Next, set the size for the mesh. Finally, mesh the midsurface.
Assigning Mesh Attributes What Assign the mesh attributes to the surfaces.
How Step
UI
Command/Display
1.
Geometry, Midsurface, Assign Mesh Attributes Menu
2.
Entity Selection dialog box: Select All OK
3.
Define Material - ISOTROPIC dialog box: Load Pick a AISI 4340 Steel. OK (all dialog boxes)
Meshing the Model
Step
UI
14-9
Command/Display Tip: If midsurfaces are created manually using commands such as Geometry, Surface, Offset or Geometry, Surface, Extrude, the surfaces do not have mesh attributes. You must manually assign mesh attributes by creating or assigning existing properties using the correct thickness.
Meshing the Model What Set the mesh size to the default value, and mesh the model.
How Step
UI
Command/Display
1.
Mesh, Mesh Control, Size on Surface Menu
2.
Entity Selection dialog box: Select All OK (all dialog boxes), then... Cancel
3.
Mesh, Geometry, Surface Menu
4.
Entity Selection dialog box: Select All OK
5.
Automesh Surfaces dialog box: Quads OK
14-10 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
Applying Loads and Constraints To load the model, you will apply a pressure to the surface at the back of the part. You will also constrain the holes at the base.
What Create a load set, the apply a pressure to the back of the part.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
Enter a name for the load set OK 2.
Model, Load, On Surface Menu
3.
Entity Selection dialog box: ID: 185 OK Notice: Surface 185 is the middle surface at the back of the part.
4.
Create Loads on Surfaces dialog box: Pressure
5.
Pressure: Value: -1 OK
Applying Loads and Constraints
Step
UI
14-11
Command/Display
V1 L1 1.1. 1. 1. 1. 1.1. 1. 1. YZ X What Constrain the holes at the bottom of the part.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
Enter a name for the constraint set OK 2.
Model, Constraint, On Curve Menu
3.
Entity Selection dialog box: Pick the eight curves around the holes at the base. OK Tip: You may want to rotate the model and zoom in on the corners of the model to make selection of these curves easier. While in a command you can use the middle mouse button to rotate the model as well as the Zoom and Previous Zoom icons on the View Toolbar.
4.
Create Constraints on Geometry dialog box: Pinned - No Translation OK
14-12 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
V1 L1 C1 TT TT Y ZX Tip: To see the nodes on which the loads and constraints are applied, use the Model, Load, Expand and Model, Constraint, Expand commands.
Analyzing the Model Solve the model using the NX Nastran solver.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Create an analysis set.
2
Analysis Program: 36..NX Nastran Analysis Type: 1..Static OK
3.
Analyze
Post-processing the Results For this analysis, you will display deformation and stress contours.
What Display and deformed/contour plot of translation and stress.
Post-processing the Results
14-13
How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Vectors: Deformation: 1..Total Translation Output Vectors: Contour: 7026..Plate Top MajorPrn Stress OK (all dialog boxes)
5. 6.
Ctrl-Q
View Quick Options Geometry Off UNCHECK Node in the Mesh Section Done
7.
Rotate the model so that you can see the back.
Notice: You can see the plate top stress contour on both faces of the plate elements.
14-14 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
What Change the contour options to display double-sided planar contours. If you select a standard top or bottom plate vector for contouring, as you did above, FEMAP can automatically contour both top and bottom stresses on the same plot. How Step
UI
Command/Display
1.
F5 key
View Select
2.
View Select dialog box: Deformed and Contour Data
3.
Select PostProcessing Data dialog box: Contour Options
4.
Select Contour Options dialog box: Contour Type: Elemental
5.
Data Conversion: Average
6.
Data Conversion: Use Corner Data
Post-processing the Results
Step 7.
UI
14-15
Command/Display Other Options: Double-Sided Planar Contours OK (all dialog boxes) Notice: The display has changed. The contour now shows plate top major principle stress on the top face of the plate elements and plate bottom major principle stress on the bottom face of the plate elements.
8.
Rotate the model to look at the back.
Notice: The contour on the back of the part shows plate top major stress.
14-16 Step
UI
Analyzing a Midsurface Model of an Electrical Box
Command/Display
What To more easily see double-sided results, change the view to show the element thicknesses.
How Step
UI
Command/Display
1.
F6 key
View Options
2.
View Options dialog box: Options: Element - Orientation/Shape, then... Element Shape: Show Fiber Thickness Tip: You can also “toggle” the thickness of planar elements on/off using the “Thickness/ Cross Section” command from the View Style menu located on the View Toolbar.
3.
Tools and View Style
4.
Filled Edges
5.
UNCHECK Draw Entity OK
Post-processing the Results
Step
UI
14-17
Command/Display Tip: You can also toggle the “Filled Edges” on and off very easily using the View Style menu located on the View Toolbar. Simply select Filled Edges from the View Style menu to turn them off, then select the command again to turn them back on at any time. Notice: The stress is now shown through the element thickness.
This is the end of the example. You don’t need to save your model file.
14-18
Analyzing a Midsurface Model of an Electrical Box
Direct Transient Analysis – Hinge Model 15.
Dynamic Analysis is used when a structure undergoes loading that occurs over time as opposed to static analysis which only takes into account the behavior of a structure at one time step. In many ways dynamic analysis is a more realistic type of analysis as compared to static analysis, but is also more complex. The loading is applied as a function of time during dynamic analysis, therefore, responses to the loading such as displacements, velocities, accelerations, forces, and stresses are also time-varying. For our first exploration of dynamic analysis, we will look at Direct Transient Analysis. Direct Transient Response can be used to determine a structure’s response to a time-varying excitation where all of the applied forces are known for each instant of time. In many cases, the desired responses to be computed are nodal displacements and accelerations, as well as, element forces and stresses.
Hinge Bracket
For this example we will be using a model of a hinge bracket that has already been created. You will work through the entire analysis process which includes:
· creating a loading function to represent sinusoidal excitation
· applying loads and constraints
· analyzing the model using NX Nastran
· post-processing the results using XY plotting capabilities
15-2
Direct Transient Analysis – Hinge Model
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/hinge.neu Locate hinge.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Creating the Dynamic Loading Function
Importing the Model
15-3
In order for the loading to be time dependent we must create a function to represent a sine pulse loading condition.
What Create a function to be used for applying a dynamic load How
Step 1.
UI
Command/Display Model, Function
Menu
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu).
2.
In Function Definition dialog box:
3.
Type “200 Hz sinusoidal pulse” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Equation radio button
15-4 5.
Direct Transient Analysis – Hinge Model
Enter the following values in the corresponding fields:
X = 0.0 To X = 0.005 Delta X = (0.005/8) Y = sin(360*200*!x)
Notice: The equation used in the Y field uses a formula creation syntax that FEMAP can read. For example the “sin” portion of the equation is telling FEMAP to take the sine of the value that is in the parenthesis (). The “!x” represents the variable x value as x increases from 0.0 to 0.005 based on the Delta X value (0.005/8 = 0.000625 for this example which will give us the needed 8 data points for our sine wave). The “200” value is our frequency in Hz. Click More button
6.
X and Y Values will be created for the function.
We need to “Zero” the curve after one single pulse, therefore we need to add one point with a “zero” Y value and a X value larger than 0.005
7.
Notice: NX/NASTRAN will use the curve coordinates for interpolation purposes and this is why the “zero” point must be added. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X =.0055 Click OK, then…
Y = 0.00
Click Cancel What Verify the function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Importing the Model
15-5
2.
In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..200 Hz sinusoidal Pulse” from Select drop down menu located in the Function portion of the window Click OK button
In View Select dialog box:
Click OK button Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key) The XY Plot should show a sine wave which levels off at the right hand side as shown below.
15-6
Direct Transient Analysis – Hinge Model
Creating the Transient Load What Apply the transient load to the hinge bracket
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose the Draw Model radio button Click OK
4.
The model should be on the screen again at this point. Model, Load, Set Menu
5.
In Create or Activate Load Set dialog box:
6.
Type “Transient Load” in the Title field Click OK
7.
Model, Load, Nodal Menu
8.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 44 at bottom right of structure
from the View Toolbar
Defining the Transient Analysis Parameters
15-7
Node 44
9.
Click OK
10.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 11.
Enter “75” into the FZ field
12.
Select “1..200 Hz Sinusoidal Pulse” from the Time/Freq Dependence drop down menu
13.
Click OK, then…
Click Cancel
Defining the Transient Analysis Parameters In order for NX Nastran to perform a direct transient analysis, there are certain parameters which must be defined within the Load Set. This will allow NX Nastran to know the number of desired time steps (each time step will produce an individual results set), the output interval, as well as, take into account the effects of damping. What Define the Dynamic Analysis Parameters
How
Step 1.
UI Menu
Command/Display Model, Load, Dynamic Analysis
15-8
Direct Transient Analysis – Hinge Model
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Direct Transient radio button Enter the following values in the corresponding fields:
Overall Structural Damping Coefficient (G) = 0.2 Frequency for System Damping (W3) = 90 Number of Steps = 99 (100 results sets produced including t=0) Time per Step = 0.0005 Output Interval = 1
4.
Notice: The Overall Structural Damping Coefficient (G =2 * (critical damping ratio)), therefore the system will experience 10% equivalent viscous damping. The Frequency for System Damping value of 90 was chosen because it is the first fundamental bending mode of this structure (This value is obtained from a normal modes analysis). The output interval of 1 will create an output set in the results file for every time step that is calculated, a value of 2 would create an output set for every other time step that NX Nastran calculates, and 3 would be every third time step and so on. Click OK
Creating the Constraints The model needs to be constrained for this example
What Create a constraint set and apply fixed nodal constraints
Defining the Transient Analysis Parameters
15-9
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Hole fixed” in the Title field Click OK button
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the nodes around the edge of the hole. This can be done by selecting one node at a time or… by holding down the Control (Ctrl) key and clicking near the center of the circle and dragging the mouse out which will create a circular picking window. Once all of the nodes are inside the circular picking window let go of the mouse button and all the nodes will be selected.
Notice: Holding down the Shift Key can also create a rectangular picking area and other picking options such as polygon, freehand, and query are available by pressing the “Pick” button inside any Entity Selection dialog box.
Nodes to be constrained
15-10 6.
Direct Transient Analysis – Hinge Model
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed Button, then…
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Setting up the Analysis Set Manager It is possible to save multiple Analysis Sets or “Cases” along with your FEMAP model. This will enable you to create multiple Analysis Cases and then select the appropriate case to be submitted to NX Nastran. For example, you can set-up one case to perform a Static analysis, one for Modal Analysis, another for Direct Transient Analysis, and yet another for Heat Transfer. All the cases can be saved with one model along with the different boundary conditions required for each separate analysis in separate load and constraint sets. You can also submit jobs to NX Nastran directly from the case manager by pressing the Analyze button.
What Create an analysis case for Direct Transient Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
Setting up the Analysis Set Manager
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Direct Transient Case” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
15-11
Select “3..Transient Dynamic/Time History” from the Analysis Type drop down menu
5.
Click OK
15-12
Direct Transient Analysis – Hinge Model
Advanced Nastran Notice: There are many NX Nastran options that can be selected and then saved using the Analysis Set Manager. These options include NASTRAN Executive and Solution controls, Bulk Data options, Element Quality Checks, Overall Model Checks, Specific Analysis Type Options, selection of Boundary Condition sets, Output Requests, and many others. The dialog boxes for each “group” of options can be reached by pressing the Next button on the Analysis Set dialog box, selecting the desired options in that specific dialog box, and then pressing the Next button again to progress to the next group of options.
For this particular example we will be using the defaults, so it is not required to alter these options to perform this analysis. Advanced Nastran Notice: For users familiar with any Nastran solver who would like to visually inspect the input deck before it is sent to the solver this can be accomplished by clicking the Preview Input button in the Analysis Set Manager dialog box. This will bring up a text viewer containing the Nastran input deck, and the viewer can become an editor by checking the box under Edit Preview. In Analysis Set Manager dialog box:
6.
Click Analyze button The Analysis should now be running, when it is complete results will be available for post-processing.
Post-Processing the Results In many cases, the results of Dynamic Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the response of a single node across the entire time history of the analysis. For this example we will use the loaded node, node number 44.
What Create a XY Plot of response of a single node of the structure
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
on the View Toolbar
Post-Processing the Results
4.
15-13
In Select XY Curve Data dialog box:
Select “1..Case 1 Time 0.” from drop down menu located in the Output Set section, then…
5.
Select “4..T3 Translation” from drop down menu located in the Output Vector section Enter “44” in the Node field located in the Output Location section
6.
In the Show Output Sets section, leave the From and To fields blank (By leaving these fields blank, the results at all output sets will be shown) Click OK, then…
In View Select dialog box:
Click OK The XY Plot the Z-translation of Node 44 should appear like this:
The XY Plot can be manipulated to take a closer look at a certain portion of the plotted response. The largest deflections of the loaded Node 44 occur between 0 and 0.03 on the X-Axis (Time), therefore we will change the range of the X-axis in order to zoom in on this part of the plot.
15-14
Direct Transient Analysis – Hinge Model
What Change the range of the X-axis on the XY Plot of Node 44
How
Step 1.
UI
Command/Display View, Options or…
Menu
2.
3.
4.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
Choose PostProcessing radio button under Category Highlight “XY X Range/Grid” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Max Min” from the Axis Range selection list Enter the following Values in the corresponding fields: Minimum = 0.0 Maximum = 0.03
5.
on the View Toolbar
Click OK
Post-Processing the Results
15-15
The Plot should now appear like this:
This Concludes the Direct Transient Analysis example. It is your choice whether or not to save the model file.
15-16
Direct Transient Analysis – Hinge Model
Modal Frequency Analysis of the Hinge Model 16.
Modal Frequency Response Analysis is used to determine a structure’s response to harmonic (oscillatory) excitation where all forces at each forcing frequency are known and defined within a frequency domain. The responses consist of complex numbers defined as magnitude and phase or as real and imaginary components.
First a Normal Modes Analysis will be run on the Hinge model to determine the natural frequencies. By using an NX Nastran option which allows analysis restarts, we will then perform a modal frequency response analysis without extracting the normal modes again. The purpose of this example is to determine the hinge structure’s response to a loading of unit amplitude across a frequency range up to 600 Hz. This frequency range has been chosen based on a prior normal modes analysis and contains the first three modes of the structure. We will assume the critical damping of the system to be 10%.
For this example we will be using a model of a hinge bracket that has already been created. You will work through the entire analysis process which includes:
· utilizing analysis restarts in NX Nastran to increase solution efficiency
· creating functions to define unit amplitude for frequency response loading and modal damping table
· analyzing the model using NX Nastran Frequency/Harmonic Response solution
· post-processing the results data using XY plotting capabilities
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI Menu
Command/Display File, New
16-2 2.
Modal Frequency Analysis of the Hinge Model
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/hinge.neu Locate hinge.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Creating the Constraints The model needs to be constrained for this example
What Create a constraint set and apply fixed nodal constraints
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Running the Normal Modes Analysis
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Hole fixed” in the Title field Click OK
4.
16-3
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples.
Nodes to be constrained
6.
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
Running the Normal Modes Analysis
16-4
Modal Frequency Analysis of the Hinge Model
Extracting the normal modes will enable NX Nastran to select solution frequencies automatically in order to create a solution frequency function. We will also take advantage of the analysis restarts option to transition from normal modes analysis to frequency response analysis.
What Create an analysis case for Normal Analysis and specify analysis restarts using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Normal Modes Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “2..Normal Modes/Eigenvalue” from the Analysis Type drop down menu
5.
Click Next
6.
In NASTRAN Executive and Solution Options dialog box:
CHECK Save Databases for Restart box in the Restart Control section
Notice: Make sure the files that NX Nastran will be using for the Restart are in a directory where none of the directory names has a space in it. For Example: If the path to the *.MASTER would be C:\Analysis Files\filename.MASTER, NX Nastran will not be able to get to the restart file. A path such as C:\Analysis_Files\filemane.MASTER would be able to be run because the directory name has an underscore instead of a space.
Creating Unit Load for Frequency Response Loading
7.
16-5
Click OK
In Analysis Set Manager dialog box:
Click Analyze button IMPORTANT: Once the Normal Modes Analysis has been completed, verify that results have been retrieved from NX Nastran by pressing the F5 key (View Select command) and then clicking the “Deformed and Contour Data” button. In the Select Post Processing dialog box under Output Set make sure “1.Mode 1, 89.81622 Hz” is visible (If there are no results, then the analysis may not have completed successfully and therefore the model should be checked for mistakes and then rerun). Click OK and OK again.
Also be sure that the NX Nastran databases (the *.MASTER and *.DBALL files, “*”denotes the filename the user has given to this example when saved before running the analysis) have been saved for “Restart” purposes in the directory where the analysis has taken place (should be in the same directory as where the results files, *.op2 and *.f06, can be found).
Creating Unit Load for Frequency Response Loading A Unit Load must be created to remain constant across the entire frequency range. A simple function will be used to represent the temporal portion of the load and then given a direction to represent the spatial portion of the loading condition.
What Create a function for the Unit Load
16-6
Modal Frequency Analysis of the Hinge Model
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Load Value vs. Frequency” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 1, Then…Click More button X = 1, Y = 1 Click OK, then...
6.
Click Cancel
What Apply the 1.0 unit load to the hinge bracket
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
Type “Unit Load” in the Title field
Creating Unit Load for Frequency Response Loading
3.
16-7
Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 44 at bottom right of structure
Node 44
6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “1.0” into the FZ field
9.
Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
10.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel The Frequency Response Loading Condition has now been applied.
Modal Damping Definition
16-8
Modal Frequency Analysis of the Hinge Model
A simple function must be created to represent the modal damping of the system. The type of function created depends on the units of the assumed damping value:
1. If the structural damping coefficient (G) is known, then Function Type “6..Structural Damping vs. Freq” should be used.
2. If the critical damping ratio is known, then Function Type “7..Critical Damping vs. Freq” should be used.
3. If the Quality/Magnification Factor (Q) is known, then Function Type “8..Q Damping vs. Frequency” should be used.
In our case, a critical damping ratio of 10% across the frequency range is desired. Therefore, we will use the Function Type “7..Critical Damping vs. Freq”. What Create a function to represent the desired Critical Damping for the system.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Damping Function” in the Title field Select “7..Critical Damping vs. Freq” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0.1, Then…Click More button
6.
X = 1, Y = 0.1 Click OK, then...
Click Cancel
Defining Solution Frequencies
Creating Unit Load for Frequency Response Loading
16-9
Solution Frequencies can be defined two separate ways. One way is to create a function which gradually raises the frequency in defined increments in a given frequency range. If you have not extracted the normal modes in a previous analysis, this is a way to create a frequency table to excite the structure. The disadvantage of this method is that it will give you a large number of data points to review in general and not concentrate the results around the natural modes, where the response should be the highest.
Because we have run a normal modes analysis, and NX NASTRAN has the Analysis Restart capability we set-up earlier, we can use a different and more effective method to create our frequency table. Utilizing the known results of the normal modes analysis we ran earlier in the tutorial, FEMAP can create a much more accurate frequency table for Modal Frequency Response. The frequency table, along with other parameters, must be defined within the Load Set before the Hinge model can be analyzed.
What Define the Frequency Table and Modal Frequency Response parameters
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Modal Frequency radio button Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section
4.
Click Modal Freq...button
5.
In Frequency Table From Modal Results dialog box:
Select “1..Mode 1, 89.81622 Hz” from the First Freq drop down menu, then…
6.
Select “3..Mode 3, 568.1597 Hz” from the Last Freq drop down menu Enter the following values into the corresponding fields:
Number of Point per Existing Modes = 5 Frequency Band Spread = 10 (%)
Notice: These values, 5 per Existing Mode and 10% Frequency Band Spread, are somewhat standard for creating the Frequency Table using existing Normal Modes.
16-10
7.
Modal Frequency Analysis of the Hinge Model
Click OK
In Load Set Options for Dynamic Analysis dialog box:
8.
Make sure “3..Modal Frequency Table” appears in the Frequencies drop down menu in the Frequency Response section. Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
Notice: The Overall Structural Damping Coefficient (G) does not need to be defined because we have already taken care of this with the function created for the Modal Damping Table.
Creating Unit Load for Frequency Response Loading
9.
16-11
Click OK
Visual verification of the Frequency Table function in a XY Plot is always a good check before analyzing the model.
What Verify the Frequency Table function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “3..Modal Frequency Table” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key)
16-12
Modal Frequency Analysis of the Hinge Model
The XY Plot should show three peaks, one peak for each of the first three modes. The Y value is arbitrary on this plot, but the x-values are an excellent way to visualize where the excitations are occurring with respect to the frequency range. Also, the width of the base of each peak represents the frequency bandwidth associated with each forcing frequency.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Modal Frequency Response Analysis What Create an analysis case for Modal Frequency Response Analysis and specify analysis restarts using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
Enter “Modal Frequency Response Analysis” in the Title field
Running the Modal Frequency Response Analysis
4.
16-13
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
5.
Click Next
6.
In NASTRAN Executive and Solution Options dialog box:
7.
CHECK Restart Previous Analysis box in the Restart Control section Click the Browse button (“...” button) and locate the “*.MASTER” file that was created earlier in the tutorial. Remember, this should be located in the same directory as your Normal Modes Analysis Results File. Then…
Click Open
16-14 8.
Modal Frequency Analysis of the Hinge Model
Click OK
In Analysis Set Manager dialog box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the response of a single node across the entire frequency range of the analysis. For this example we will use the loaded node, node number 44.
What Create a XY Plot of response of a single node of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
from the View Toolbar
Select “11..Case 1 Freq 80.83459” from drop down menu located in the Output Set section, then…
5.
Select “4..T3 Translation” from drop down menu located in the Output Vector section Enter “44” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “25” in the To field in the Show Output Sets section
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the frequency response of Node 44.
Post-Processing the Results
6.
16-15
Click OK, then…
In View Select dialog box:
Click OK The resulting XY Plot will show the Z-Translation of Node 44 across the entire frequency range.
This concludes the Modal Frequency Response Analysis example. Please save this model as Hingemodal.mod for use in a later tutorial.
16-16
Modal Frequency Analysis of the Hinge Model
Frequency Response of Tower with Seismic Excitation 17.
This example will move step by step through a Frequency Response Analysis of a tower being forced at a base node with a 1g sinusoidal (Seismic) loading condition. The model of the tower has been constructed and a modal analysis has been run previously. We will import the model and concentrate on the creation of Frequency Response loading conditions, the two different methods of applying the excitation to the model (Large Mass and Direct Methods), and post-processing the results of the analysis by examining accelerations of specific nodes.
Large Mass Method
Direct Method
For this example we will be using a model of a communications tower that has already been created. You will work through the entire analysis process which includes:
· creating a loading condition to represent a seismic excitation
· applying loads and constraints specific to both methods of creating the excitation
· analyzing the model using NX Nastran
· post-processing the results using multiple curves in XY plots.
17-2
Frequency Response of Tower with Seismic Excitation
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Dynamics/tower.neu Locate tower.neu
Click Open
Neutral File Read Options dialog box:
Click OK
View the results of Modal Analysis
Importing the Model
17-3
What View an animation of the Mode Shapes created by the Natural Frequencies
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate radio button in the Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Mode 1, 10.8234 Hz” from the drop down menu in the Output Set section
Select “1..Total Translation” from Deformation drop down menu in the Output Vector section Click OK
5.
In View Select dialog box:
Click OK
The Model should now be moving based on the first Natural Frequency.
What Change the Output Set (Mode Shape) being viewed a few different ways
How You can follow Steps 1-3 above, then Select “The mode you want to view” from the drop down menu in the Output Set section, then follow Steps 5-6.
OR
Step
UI
Command/Display
17-4
Frequency Response of Tower with Seismic Excitation
1.
Click the Right Mouse button and highlight Post Data
2.
In Select PostProcessing Data dialog box:
3.
Select “The mode you want to view” from the drop down menu in the Output Set section Click OK
OR
Step 1.
UI Menu
Command/Display Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) This will bring up the Post Toolbar.
Click the Next Set icon or the Previous Set icon to move back and forth through the existing Output Sets (These icons are located on the Post Toolbar)
Notice: The Toolbars contain many popular commands that can be accessed in one click or choosing off a short menu instead of through multiple cascading menus and/or dialog boxes. Take some time to become familiar with some of the features conveniently located on the Command Toolbar.
After all of the Mode Shapes have been viewed:
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose None-Model Only radio button in the Deformed Style section Click OK
Modal Damping Definition
from the View Toolbar
Creating Function for Seismic Loading
17-5
A simple function must be created to represent the modal damping of the system. The type of function created depends on the units of the assumed damping value:
What Create a function to represent the desired Critical Damping for the system.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Damping Function” in the Title field Select “7..Critical Damping vs. Freq” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0.1, Then…Click More button
6.
X = 1, Y = 0.1 Click OK, then...
Click Cancel
Creating Function for Seismic Loading A Function must be created to remain constant across the entire frequency range. A simple function will be used to represent the temporal portion of the load and then given a direction and magnitude to represent the spatial portion of the loading condition later in the example
What
17-6
Frequency Response of Tower with Seismic Excitation
Create a function for the Seismic Loading
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “1g Loading” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 1, Then…Click More button
X = 1, Y = 1 Click OK, then...
6.
Click Cancel
Defining Solution Frequencies
As in our Modal Frequency Example 16 we will create our Solution Frequency Table using our existing Modal Analysis.
What Define the Frequency Table and Modal Frequency Response parameters
How
Step 1.
UI Menu
Command/Display Model, Load, Set
Creating Function for Seismic Loading
2.
In Create or Activate Load Set dialog box:
3.
Type “Seismic Load” in the Title field Click OK
4.
17-7
Model, Load, Dynamic Analysis Menu
5.
In Load Set Options for Dynamic Analysis dialog box:
6.
Choose Modal Frequency radio button Select “1..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section
7.
Click Modal Freq...button
8.
In Frequency Table From Modal Results dialog box:
Select “1..Mode 1, 10.8234 Hz” from the First Freq drop down menu, then…
9.
Select “5..Mode 5, 28.03074 Hz” from the Last Freq drop down menu Enter the following values into the corresponding fields:
Number of Point per Existing Modes = 5 Frequency Band Spread = 10 (%)
Notice: These values, 5 per Existing Mode and 10% Frequency Band Spread, are somewhat standard for creating the Frequency Table using existing Normal Modes.
17-8 10.
Frequency Response of Tower with Seismic Excitation
Click OK
In Load Set Options for Dynamic Analysis dialog box:
Make sure “3..Modal Frequency Table” appears in the Frequencies drop down menu in the Frequency Response section. Enter the following values in the corresponding fields:
11.
Highest Freq (Hz) = 200
Notice: The Overall Structural Damping Coefficient (G) does not need to be defined because we have already taken care of this with the function created for the Modal Damping Table. Click OK
12.
Creating the Base Node and Rigid Connection What Create the Base Node (Node which will have excitation applied)
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Enter the following values into the corresponding fields:
3.
X = 0, Y = -220, Z = 0 Click OK, then…
Click Cancel
What Create Rigid Connection between Base Node and Tower
How
Creating the Base Node and Rigid Connection
Step 1.
UI
17-9
Command/Display Model, Element
Menu
2.
In the Define PLATE (or “Type of Element”) Element – Enter Nodes or Select with Curser dialog box:
3.
Click Type button In the Element/Property Type dialog box:
4.
Choose Rigid radio button in the Other Elements section Click OK
5.
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
6.
Choose the newly created node located below the tower (node 269) for the node in the Independent section UNCHECK the RX, RY, and RZ boxes in the Independent section
7.
Click Nodes button in the Dependent portion of the dialog box
8.
In the Entity Selection – Select Master Node(s) dialog box:
Select the node at the bottom of each “leg” of the tower (nodes 50, 61, 67, and 78)
Nodes to be selected 9.
Click OK
17-10
10.
Frequency Response of Tower with Seismic Excitation
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
Click OK, then…
Click Cancel IMPORTANT: At this point the exercise will have two separate sections. One section will cover the “Large Mass Method” and the other will cover the “Direct Method” of creating a seismic loading condition. Please give both methods a try. Save your model at this point as tower.mod, in order to have a good starting point for the two separate sections.
Large Mass Method Creating the Seismic Mass
What Create Mass Property and then Mass Element
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In the Define Property – RIGID (or “Type of Element”) Element Type dialog box:
3.
Click Elem/Property Type button In the Element/Property Type dialog box:
4.
Choose Mass radio button in the Other Elements section Click OK
Large Mass Method
5.
In the Define Property – MASS Element Type dialog box:
Type “Base Mass” in the Title field
Enter “1.0E13” in the Mass, M or Mx field
6.
Click OK, then…
7.
Click Cancel Model, Element Menu
8.
In Define MASS Element – Enter Node or Select with Cursor dialog box:
Select the Base Node (Node 269) 9.
Select “3..Base Mass” from the Property drop down menu
10.
Click OK, then…
Cancel Creating the Load and Permanent Constraints
What Create Load for Large Mass
17-11
17-12
Frequency Response of Tower with Seismic Excitation
How
Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Base Node (node 269) 3.
Click OK
4.
In the Create Loads on Nodes dialog box:
Highlight Force from the selection list 5.
Enter “386.4E13” into the FX field
6.
UNCHECK the FY and FZ boxes
7.
Select “2..1g Loading” from the Time/Freq Dependence drop down menu
8.
Click OK, then…
Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
What Create Permanent Constraints on the Base Node
How
Step 1.
UI
Command/Display Modify, Edit, Node
Menu
2.
Entity Selection – Select Node(s) to Edit dialog box:
Select the Base Node (node 269)
Running the Seismic Analysis
3.
17-13
Click OK, then…
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click Parameters button In the Node Parameters dialog box:
4.
CHECK the TY, TZ, RX, RY, and RZ boxes in the Permanent Constraint section
Notice: This will create Permanent Constraints on the Node Entry in the NX NASTRAN input file (GRID,269,0,0.,-220.,0.,0,23456). These type of constraints do not require a defined constraint set, NX NASTRAN understands that this particular node is constrained in the 23456 degrees of freedom for any analysis regardless of other Constraint Sets. Click OK, then…
5.
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click OK THE MODEL IS NOW READY TO BE ANALYZED!
Running the Seismic Analysis What Create an analysis case for Seismic Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager Dialog Box:
3.
Click New button In Analysis Set Dialog Box
Type “Seismic Analysis” in the Title field
17-14 4.
Frequency Response of Tower with Seismic Excitation
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
5.
Click OK
In Analysis Set Manager Dialog Box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the nodal accelerations of a few nodes across the entire frequency range of the analysis. For this example we will use the view the accelerations at node numbers 75, 249, and 151.
What Create a XY Plot of the responses of multiple nodes of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
from the View Toolbar
Post-Processing the Results
4.
17-15
In Select XY Curve Data dialog box:
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
5.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “75” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
6.
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the accelerations. Choose “2” radio button in the Curve section
7.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
8.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “249” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
9.
Enter “35” in the To field in the Show Output Sets section Choose “3” radio button in the Curve section
10.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
11.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “151” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
12.
Enter “35” in the To field in the Show Output Sets section Click OK, then…
In View Select dialog box:
Click OK
17-16
Frequency Response of Tower with Seismic Excitation
The XY Plot of the accelerations at nodes 75, 249, 151 should look like this:
This concludes the Seismic Analysis using the Large Mass Method section of the example. Please save this model as TowerLMM.mod. Please open the Tower.mod model that you saved earlier in the example and we will now complete the analysis using the Direct Method.
Direct Method Creating the Load and Permanent Constraints
What Create Acceleration Load
How
Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Base Node (node 269) 3.
Click OK
Direct Method
4.
In the Create Loads on Nodes dialog box:
Highlight Acceleration from the selection list 5.
Enter “386.4” into the AX field
6.
UNCHECK the AY and AZ boxes
7.
Select “2..1g Loading” from the Time/Freq Dependence drop down menu
8.
Click OK, then…
Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Create constraints on the Base Node
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed Base Node” in the Title field Click OK button
4.
Model, Constraint, Nodal Menu
5.
In Entity Selection – Enter Node(s) to Select dialog box
Select the Base Node (Node 269)
17-17
17-18 6.
Frequency Response of Tower with Seismic Excitation
Click OK, then...
In Create Nodal Constraints/DOF dialog box:
Click the Fixed Button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Seismic Analysis What Create an analysis case for Seismic Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Seismic Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “4..Frequency/Harmonic Response” from the Analysis Type drop down menu
Post-Processing the Results
5.
Click Next button 2 times, then…
6.
In NASTRAN Bulk Data Options dialog box:
17-19
CHECK the box next to RESVEC (make sure it also is set to “On”)
Notice: It is highly recommended during Frequency Response where the Direct Method is used that the Residual Vector Parameter (RESVEC) be used for increased solution accuracy. Click OK, then…
7.
In Analysis Set Manager dialog box:
Click Analyze button
Post-Processing the Results In many cases, the results of Modal Frequency Analysis are best viewed utilizing the XY Plotting capabilities of FEMAP. We will examine the nodal accelerations of a few nodes across the entire frequency range of the analysis. For this example we will use the view the accelerations at node numbers 75, 249, and 151.
What Create a XY Plot of the responses of multiple nodes of the structure over the frequency range
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
17-20
Frequency Response of Tower with Seismic Excitation
2.
In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
5.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “75” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
6.
Notice: The first 10 output sets in the model represent the normal modes of the structure and should not be included in a plot of the accelerations. Choose “2” radio button in the curve section
7.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
8.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “249” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
9.
Enter “35” in the To field in the Show Output Sets section Choose “3” radio button in the curve section
10.
Select “11..Case 1 Freq 9.74106” from drop down menu located in the Output Set section, then…
11.
Select “22..T1 Acceleration” from drop down menu located in the Output Vector section Enter “151” in the Node field located in the Output Location section
Enter “11” in the From field in the Show Output Sets section
Enter “35” in the To field in the Show Output Sets section
Post-Processing the Results
12.
Click OK, then…
In View Select dialog box:
Click OK The XY Plot of the accelerations at nodes 75, 249, 151 should look like this:
This concludes the Seismic Analysis example. Please save this model as TowerDM.mod.
17-21
17-22
Frequency Response of Tower with Seismic Excitation
Random Response of the Hinge Model 18.
Random Frequency (Vibration) Response can be used to simulate such effects as earthquake ground motion, pressure fluctuations caused by wind on tall buildings and aircraft, and acoustic excitation due to jet and rocket engine noise. In NX Nastran, Random Response Analysis is performed as a “post-processing” to a previously completed Frequency Response Analysis. Random Response requires many of the same inputs used in Frequency Response, but also requires an additional user-defined loading condition such as a load governed by a Power Spectral Density (PSD) function.
There are two separate methods to create enforced base motion to excite the structure using NX Nastran. The first method is the “Large Mass method” which requires a load, such as a force, be applied to a “large mass” attached to the structure, which in this case will simulate an acceleration load. A Large Mass is described as an object (usually a single point mass) between 105 and 1013 times the mass of the structure. The other method is quite a bit easier to set-up and allows the user to apply the nodal load directly to a specific node and does not require the user to create a Large Mass in order to apply enforced motion. This “Direct Method” was developed for MSC.NASTRAN version 2001 and later (This includes all version of NX Nastran), therefore it should be the preferred method for those users who are learning to perform analyses involving enforced motion. We will explore both methods in this exercise. A great resource for Random Vibration Analysis is located at: http:// analyst.gsfc.nasa.gov/FEMCI/random/
For this example, you will need to have completed the Modal Frequency Response exercise to continue because we will be using the hingemodal.mod file you have saved. You will work through the entire analysis process which includes:
· creating a Power Spectral Density (PSD) function
· creating an enforced motion loading condition using the “Large Mass Method” and the “Direct Method”
· setting up a group in order to make specific output requests
· analyzing the model using NX Nastran Random Response solution
· post-processing results functions using XY plotting capabilities
Opening an Existing FEMAP Model What Open an existing FEMAP model file hingemodal.mod.
18-2
Random Response of the Hinge Model
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Dynamics/Random Response/hingemodal.mod
Click Open
Deleting existing Loads and Boundary Conditions
What Delete Load Sets and Constraint Sets.
How
Step 1.
UI Menu
Command/Display Delete, Model, Load Set
Defining the Power Spectral Density Function
2.
18-3
In Entity Selection – Select Load Set(s) to Delete dialog box:
Click Select All button, then…
Click OK, then…
In Confirm Delete dialog box:
Click OK Delete, Model, Constraint Set
3. Menu
4.
In Entity Selection – Select Constraint Set(s) to Delete dialog box:
Click Select All button, then…
Click OK, then…
In Confirm Delete dialog box:
Click OK Tip: You can quickly delete both Load and Constraint sets from the Model Info tree. Simply highlight either the “top-level” Loads branch or the Constraints branch, then right click and choose the Delete command form the “context sensitive menu” (this will delete ALL Load or Constraint sets). This command will also work with any individual Load or Constraint Sets.
Defining the Power Spectral Density Function Power Spectral Density (PSD) functions are created from empirical data recovered by accelerometers during dynamic testing (we will actually be creating an Acceleration Spectral Density (ASD) function which approximates the actual PSD plot, but will refer to it as a PSD function). For this example we are going to use a very basic PSD function in order to demonstrate the use of a PSD function in Random Response. The Units of our PSD function are G2/Hz, where G is Gravitational Acceleration vs. Frequency in Hz.
What Create a simple PSD function
How
Step
UI
Command/Display
18-4 1.
Random Response of the Hinge Model
Model, Function Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “PSD Function” in the Title field Select “3..vs. Frequency” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 20, Y = 0.1, Then…Click More button X = 40, Y = 1.0, Then…Click More button X = 100, Y = 1.0, Then…Click More button X = 350, Y = 0.1, Then…Click More button X = 700, Y = 0.1 Click OK, then...
6.
Click Cancel Visual verification of the PSD function in a XY Plot is always a good check before analyzing the model. What Verify the PSD function using the XY Plotting Feature of FEMAP How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
Choose XY of Function radio button
from the View Toolbar
Defining the Power Spectral Density Function
18-5
3.
Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “4..PSD Function” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK
Notice: In order to create an XY plot that is more representative of a PSD function we will want to view it in as a Log-Log Plot instead of the default Rectilinear format. View, Options or…
6. Menu
7.
8.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
Choose PostProcessing radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Log-Log” from the Plot Type selection list
9.
on the View Toolbar
Click OK
18-6
Random Response of the Hinge Model
The XY Plot should now look like this:
What Change View so model can be seen for selection purposes. How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Draw Model radio button Click OK
from the View Toolbar
IMPORTANT: At this point the exercise will split into two separate sections until it is time to analyze the model. One section will cover the “Large Mass Method” and the other will cover the “Direct Method” of Enforced Motion Application. If you are familiar with the “Large Mass Method” and plan to continue using this method, please continue on with the tutorial starting below this message. If you have not done Enforced Motion analysis before, we suggest you concentrate on the “Direct Method”, which starts on page (page 18-10), with the heading “Creating Enforced Motion Loading using the Direct Method”, because it is the updated means to perform an Enforced Motion Analysis. If you would like to give both methods a try, please save your model at this point as hingePSD.mod, in order to have a good starting point for the two separate sections.
Creating Enforced Motion Loading - Large Mass Method
18-7
Creating Enforced Motion Loading - Large Mass Method What Define the Random Frequency Response parameters and create Large Mass for Enforced Motion.
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
FEMAP will prompt you to Create a Load Set.
In Create or Activate Load Set dialog box:
3.
Type “Enforced Motion” in the Title field Click OK
4.
In Load Set Options for Dynamic Analysis dialog box:
5.
Choose Modal Frequency radio button Click Enforced Motion button
6.
FEMAP will ask for the coordinates of a “Base Mass”
In the Locate – Enter Coordinates for Base Mass dialog box:
Enter the following values in the corresponding fields:
X = -0.5, Y = 4, Z = 0 (This will position a point mass at the center of the hole)
7.
Click OK
18-8 8.
Random Response of the Hinge Model
Entity Selection – Select Nodes on Base dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples. A good idea here is holding the CTRL Key, selecting near the center of the hole and dragging the picking circle out until desired nodes are within circular picking area.
Nodes to be selected for base
9.
Click OK
10.
In the Create Loads on Nodes dialog box:
11.
Highlight Acceleration from the selection list if not already selected Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
12.
Check AZ box for text field to become available
13.
Enter “1.0” into the AZ field
Creating Enforced Motion Loading - Large Mass Method
14.
Click OK
15.
In Mass/Accel Scale Factor dialog box:
18-9
Verify the following fields:
Mass = 0.0070248, Factor = 1000000.
16.
Click OK
17.
In Load Set Options for Dynamic Analysis dialog box:
Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section, then…
Select “3..Modal Frequency Table” from the Frequencies drop down menu in the Frequency Response section, then…
Select “4..PSD Function” from the PSD drop down menu in the Random Analysis Options section
18-10 18.
Random Response of the Hinge Model
Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
19.
Click OK
Notice: A Mass Element with an acceleration load connected to the nodes around the hole with a Rigid Element has been created for Enforced Motion purposes.
Rigid Element
Mass Element
What Create a constraint set to constrain the excitation node in all directions except for the acceleration direction (Z-translation).
Creating Enforced Motion Loading - Large Mass Method
18-11
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
Type “1” in the ID field
Type “Load Constraint” in the Title field Click OK
3. 4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node “289” at the center of the circle 6.
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Fixed, then… 7. UNCHECK the TZ box (leaving the rest of degrees-of-freedom checked) 8.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel
IMPORTANT: You have finished creating the Enforced Motion portion of the Random Response Analysis tutorial using the “Large Mass” method. To learn how to analyze and post-process the results of the Random Response, please move ahead to the “Creating a Group for Output Request needs” portion of the tutorial. If you would like to try using the “Direct Method” to define Enforced Motion, save your model as hingeLMM.mod and open hingePSD.mod and continue with the tutorial below.
18-12
Random Response of the Hinge Model
Creating Enforced Motion Loading - Direct Method No Large Mass is required to apply an excitation such as acceleration to an individual node when the “Direct Method” is used to define Enforced Motion.
What Create a base node and connect it to the structure with a rigid element.
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Curser dialog box:
Enter the following values in the corresponding fields:
3.
X = -0.5, Y = 4, Z = 0 (This will position a node at the center of the hole) Click OK, then…
4.
Click Cancel Model, Element Menu
5.
In the Define PLATE (or “Type of Element”) Element – Enter Nodes or Select with Curser dialog box:
6.
Click Type button In the Element/Property Type dialog box:
7.
Choose Rigid radio button in the Other Elements section Click OK
8.
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
9.
Choose the newly created node at the center of the hole (node 289) for the node in the Independent section Click Nodes button in the Dependent portion of the dialog box
Creating Enforced Motion Loading - Direct Method
10.
18-13
Entity Selection – Select Master Node(s) dialog box:
Select the nodes around the edge of the hole either one node at a time or using alternative picking methods discussed in previous examples. A good idea here is holding the CTRL Key, selecting near the center of the hole and dragging the picking circle out until desired nodes are within circular picking area (this will pick the center node, but we will remove it from the selection list in the next step)
Nodes to be selected for base
11.
Highlight “+289” from the selection list if not already selected.
12.
Click Delete, then...
Click OK, then…
In the Define RIGID Element – Enter Nodes or Select with Curser dialog box:
Click OK, then…
Click Cancel What Create an acceleration load directly on a node.
How
Step
UI
Command/Display
18-14 1.
Random Response of the Hinge Model
Model, Load, Set Menu
2.
In Create or Activate Load Set Dialog Box:
3.
Type “Acceleration Load” in the Title field Click OK button
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 289 at center of hole
Node 289
6.
Click OK
7.
In the Create Loads on Nodes dialog box
Highlight Acceleration from the selection list 8.
Enter “1.0” into the AZ field
9.
UNCHECK the AX and AY boxes
10.
Select “1..Load Value vs. Frequency” from the Time/Freq Dependence drop down menu
Setting the Random Response Parameters
11.
18-15
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel
Setting the Random Response Parameters What Define the parameters for Random Response Analysis
How
Step 1.
UI
Command/Display Model, Load, Dynamic Analysis
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Modal Frequency radio button Select “2..Damping Function” from the Modal Damping Table drop down menu in the Equivalent Viscous Damping section, then…
Select “3..Modal Frequency Table” from the Frequencies drop down menu in the Frequency Response section, then…
4.
Select “4..PSD Function” from the PSD drop down menu in the Random Analysis Options section Enter the following values in the corresponding fields:
Highest Freq (Hz) = 1000
18-16
5.
Random Response of the Hinge Model
Click OK
Creating the Constraints The node being “excited” needs to be fixed (including in the direction of the acceleration) when using the Direct Method. This is a major difference between the Large Mass Method and the Direct Method.
What Create a constraint set and apply a “fixed” nodal constraint on the excited node.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Load Constraint” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
Creating a Group for Output Request needs
5.
18-17
Entity Selection – Enter Node(s) to Select dialog box
Select the node “289” at the center of the circle 6.
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Fixed, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel IMPORTANT: The tutorial is the same for both Enforced Motion Methods from this point except for one small difference which is documented in the “Running the Random Response Analysis” section.
Creating a Group for Output Request needs What Create a group containing a node in order to recover specific, requested output responses.
How
Step 1.
UI
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Results Nodes” in the Title field Click OK
4.
Group, Node, ID Menu
5.
In Entity Selection – Select Node(s) for Group dialog box:
Enter “44” into the ID field
18-18 6.
Random Response of the Hinge Model
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Random Response Analysis What Create an analysis case for Random Response Analysis and specify output requests using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Random Response” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “6..Random Response” from the Analysis Type drop down menu
5.
If you are using a previous version of NX Nastran for FEMAP (versions 8.3 to 9.1) and are using the “Direct Method” for this example, please read the notice below. There is a different process you will want to follow to get accurate results. If you used either method in NX Nastran for FEMAP version 9.2 or above, then simply... Click Next button 8 times
Running the Random Response Analysis
18-19
Notice: DO NOT DO THIS STEP IF YOU ARE USING THE LARGE MASS METHOD IN ANY VERSION OF NX NASTRAN FOR FEMAP OR THE DIRECT METHOD IN NX NASTRAN VERSION 9.2 OR HIGHER. It is not required for NX Nastran 4.1, which is in version of NX Nastran in FEMAP version 9.2. Click Next button 2 times, then in the NASTRAN Bulk Data Options dialog box, Check the box next to RESVEC, then…
Click Next button 6 times
6.
It is highly recommended during dynamic response analysis where enforced motion is employed using the Direct Method that the Residual Vector Parameter (RESVEC) be used for increased solution accuracy. In NASTRAN Output for Random Analysis dialog box:
CHECK both “T3” boxes for Displacement and Acceleration in the Nodal Output Request section (This will request XY data for the node across the frequency range)
7.
Click OK
8.
In Nodal Results dialog box:
Highlight “1..Results Nodes” from the Group selection list
18-20
Random Response of the Hinge Model
9.
Click OK
10.
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read PSD vs. Frequency Functions?”...Click Yes
Post-Processing the Random Response Analysis We have requested XY plotted data (PSD vs. Frequency functions) for the nodal acceleration and displacement for the node that we placed in our “Results Nodes” group. FEMAP will create functions representing this data. This data is available in the *.f06 print results file and NOT the *.op2 binary results file. Make sure to read in the *.f06 file in order to view the requested output.
What View the Acceleration results function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
from the View Toolbar
Select “6..ACC3 PSD Node 44” from Select drop down menu located in the Function portion of the window
Post-Processing the Random Response Analysis
5.
18-21
Click OK
In View Select dialog box:
Click OK View, Options or…
6. Menu
7.
8.
9.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “0..Rectilinear” from the Plot Type selection list Click OK
The plot of the Acceleration Function of Node 44 should look like this:
This completes the Random Response example. Save the model as hingerandom.mod.
18-22
Random Response of the Hinge Model
Generation of Response Spectra Single Degree of Freedom model 19.
Response Spectrum Analysis is used to approximate the peak response to a transient excitation at the base of the structure. It is a useful tool in determining the maximum response of a structure without regard to the exact time it is occurring. For instance, the effects an earthquake might have on a specific floor of a building or a smaller component on a ship being excited by an explosion. The results of the Response Spectrum can then be applied to a specific component to determine localized results such as stress. This type of analysis is also referred to as Shock Spectrum Analysis.
A very simple model will be created in order to demonstrate the techniques used in creating a Response Spectrum.
For this example a Single Degree-of-Freedom model will be used. You will work through the entire analysis process which includes:
· creating the Single Degree-of-Freedom model
· creating a loading function to represent sinusoidal excitation, as well as, functions to represent Oscillation Frequencies and Oscillation Damping
· analyzing the model using NX Nastran
· post-processing the acceleration of the nodal results using XY plotting capabilities
Creating the Model Our will have one node and one Unit Mass element. The node will be permanently constrained in all but the x-translation degree-of-freedom.
What Creating a Node with Permanent Constraints
How
Step
UI
Command/Display
19-2 1.
Generation of Response Spectra - Single Degree of Freedom model
File, New Menu
2.
Model, Node Menu
3.
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Enter the following values into the corresponding fields:
4.
X = 0, Y = 0, Z = 0 Click Parameters button
5.
In the Node Parameters dialog box:
6.
CHECK the TY, TZ, RX, RY, and RZ boxes in the Permanent Constraint section Click OK, then…
In the Locate – Select Coordinates or Select with Cursor dialog box:
Click OK, then…
In the Locate – Enter Coordinates or Select with Cursor dialog box:
Click Cancel What Create Mass Property and then Mass Element
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In the Define Property – PLATE (or “Type of Element”) Element Type dialog box:
Click Elem/Property Type button
Creating the Dynamic Loading Function
3.
In the Element/Property Type dialog box:
4.
Choose Mass radio button in the Other Elements section Click OK
5.
In the Define Property – MASS Element Type dialog box:
19-3
Type “Base” in the Title field
6.
Enter “1.0” in the Mass, M or Mx field Click OK, then…
7.
Click Cancel Model, Element Menu
8.
In Define MASS Element – Enter Node or Select with Cursor dialog box:
Select the Node 9.
Select “1..Base” from the Property drop down menu
10.
Click OK, then…
Cancel
Creating the Dynamic Loading Function In order for the loading to be time dependent we must create a function to represent a sine pulse loading condition.
What Create a function to be used for applying a dynamic load
How
Step 1.
UI Menu
Command/Display Model, Function
19-4
Generation of Response Spectra - Single Degree of Freedom model
2.
In Function Definition dialog box:
3.
Type “200 Hz sinusoidal pulse” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Equation radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 0.005 Delta X = (0.005/8) Y = sin(360*200*!x)
Notice: This is the same function that was created in the Direct Transient example. 6.
Click More button
X and Y Values will be created for the function. A “Zero” value must be given after one single pulse, therefore we need to add one point with a “zero” Y value and a X value larger than 0.005
7.
Notice: NX Nastran will use the curve coordinates for interpolation purposes and this is why the “zero” point must be added. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X = 0.0055 Click OK, then…
Y = 0.00
Click Cancel What Verify the function using the XY Plotting Feature of FEMAP
How
Step
UI
Command/Display
Creating the Load
1.
19-5
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..200 Hz sinusoidal Pulse” from Select drop down menu located in the Function portion of the window Click OK button
In View Select dialog box:
Click OK button The XY Plot should show a sine wave shown below.
Creating the Load What Create a nodal load
How
Step
UI
Command/Display
from the View Toolbar
19-6 1.
Generation of Response Spectra - Single Degree of Freedom model
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose the Draw Model radio button Click OK
4.
The model should be on the screen again at this point. Model, Load, Set
from the View Toolbar
Menu
5.
In Create or Activate Load Set dialog box:
6.
Type “Base Excitation” in the Title field Click OK
7.
Model, Load, Nodal Menu
8.
Entity Selection – Enter Node(s) to Select dialog box:
Select Node 1 9.
Click OK
10.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 11.
Enter “1.0” into the FX field
12.
UNCHECK the FY and FZ boxes
13.
Select “1..200 Hz Sinusoidal Pulse” from the Time/Freq Dependence drop down menu
14.
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel
Creating the Load
19-7
Creating the Oscillator Functions to Generate Response Spectra
Functions for the Frequency range and the Damping values must be created in order to generate the desired results from the analysis
What Create a function for the Response Spectrum Frequencies
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Oscillator Frequencies” in Title field Select “0..Dimensionless” from Type drop down menu.
4.
Choose Equation radio button
5.
Enter the following values in the corresponding fields:
X = 20 To X = 1000 Delta X = 20
Notice: We enter nothing in the Y field, therefore generating a 0 for the Y-Value at all X-Values, which creates a frequency range. Click OK, then...
6.
Click Cancel
What Create a function for the Response Spectrum Frequencies
How
Step
UI
Command/Display
19-8 1.
Generation of Response Spectra - Single Degree of Freedom model
Model, Function Menu
2.
In Function Definition dialog box:
3.
Type “Oscillator Damping” in Title field Select “0..Dimensionless” from Type drop down menu.
4.
Choose Single Value radio button (if not already selected)
5.
Enter the following values in the corresponding fields:
X = 0, Then…Click More button X = 0.05, Then…Click More button X = 0.10
Notice: We enter nothing in the Y field, therefore generating a 0 for the Y-Value at all X-Values, which creates different damping values Click OK, then…
6.
Click Cancel
Setting the Response Spectrum Generation Parameters The number of time steps, time per step, and selection of Response/Shock Spectrum Frequencies and Damping functions must be set in order for NX Nastran to run the analysis.
What Set the parameters for Response Spectra Generation
How
Step 1.
UI Menu
Command/Display Model, Load, Dynamic Analysis
Setting the Response Spectrum Generation Parameters
2.
In Load Set Options for Dynamic Analysis dialog box:
3.
Choose Direct Transient radio button Enter the following values in the corresponding fields:
19-9
Number of Steps = 100 Time per Step = 0.0005 Output Interval = 1
4.
Notice: The Time per Step must be set to a value smaller than the time period of the sine pulse in order for the analysis to run. Select “2..Oscillator Frequencies” from the Frequencies drop down menu in the Response/Shock Spectrum section (left side of the dialog box)
Select “3..Oscillator Damping” from the Damping drop down menu in the Response/Shock Spectrum section (right side of the dialog box)
5.
Click OK
Creating a Group for Output Request needs
What Create a group containing a node in order to recover specific, requested output responses.
How
19-10
Step 1.
UI
Generation of Response Spectra - Single Degree of Freedom model
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Results Nodes” in the Title field Click OK
4.
Group, Node, ID Menu
5.
In Entity Selection – Select Node(s) for Group dialog box:
6.
Enter “1” into the ID field Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Setting up the Analysis Set Manager What Create an analysis case for Direct Transient Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
Type “Response Spectrum Gen” in the Title field
Setting up the Analysis Set Manager
4.
Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “5..Response Spectrum” from the Analysis Type drop down menu
5.
Click Next button 7 times
6.
In NASTRAN Output for Response Spectrum Analysis dialog box:
7.
Choose Absolute radio button (if not already selected) CHECK T1 box next to Acceleration
8.
Click OK
9.
In Nodal Results dialog box:
Highlight “1..Results Nodes” from the Group selection list
19-11
19-12 10.
Generation of Response Spectra - Single Degree of Freedom model
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-processing - Response Spectrum Generation We have requested XY plotted data for the nodal accelerations for the node that we placed in our “Results Nodes” group. Our Oscillator Damping function will make sure that NX Nastran produces an acceleration plot at 0%, 5%, and 10% damping conditions. FEMAP will create functions representing this data. This data is available in the *.f06 print results file and NOT the *.op2 binary results file. Make sure to read in the *.f06 file in order to view the requested output.
What View the Acceleration results function using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “5..ABSACC1 1 0.05” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK View, Options or…
6. Menu
Press the F6 Key or choose “options” from the view icon
on the View Toolbar
Post-processing - Response Spectrum Generation
19-13
7.
In View Options dialog box:
8.
Choose PostProcessing Radio button under Category Highlight “XY Axes Style” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
9.
Highlight “2..Log-Log” from the Plot Type selection list Click OK
The XY Plot of X-Acceleration at 5% damping should look like this:
This completes the Response Spectrum Generation example. Save the model as Spectrum.mod.
19-14
Generation of Response Spectra - Single Degree of Freedom model
Thermal Stress Analysis Mounting Plate 20.
Heat Transfer Analysis is used to determine the effects Conduction, Convection, and Radiation can have on a structure. Heat Transfer can occur during a Steady-Sate condition or over time with Transient Analysis. Material Properties, Heat Transfer Coefficients, and Heat Flux can be temperature dependent. Flow conditions can be set for Forced Convection, view factor calculations performed for Radiation analysis, as well as many other factors which help determine a system’s behavior when thermal conditions are involved. NX Nastran supports many options used in Heat Transfer analysis, many of which will be explored in this section of examples.
A mounting plate will be subject to a temperature of 250º F at same time another portion of the plate is being heated at 200º F. The ambient temperature of the plate and surroundings is 70º F. A temperature will be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. Those nodal temperatures will then become the loading condition for a static analysis to determine the thermal stress the mounting plate will encounter.
Mounting Plate
For this example we will be using a model of a mounting plate (with underlying geometry) that has already been created. The analysis process includes:
· creating an ambient temperature body load as well as nodal temperatures.
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· creating a load from the temperature results, as well as, defining pinned constraints
20-2
Thermal Stress Analysis - Mounting Plate
· analyzing the model with NX Nastran’s Static Solution Method and then post processing the stress results using FEMAP’s contour capabilities
Importing the Model What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Heat_Transfer/HTPlate.neu Locate HTPlate.neu
Click Open
Neutral File Read Options dialog box:
Click OK
Creating the Thermal Boundary Conditions
20-3
Creating the Thermal Boundary Conditions The model needs to have an ambient temperature set with a body load. Then localized heating in the form of nodal temperatures will also be created.
What Creating the Temperature Body Load
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Thermal” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “70” into the Default Temperature (T) field
20-4
7.
Thermal Stress Analysis - Mounting Plate
Click OK
What Creating the Nodal Temperatures using the nodes’ associativity to the underlying geometric curves
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
In View Quick Options dialog box:
CHECK Curve box located in the Geometry section, then
3.
UNCHECK Element box located in the Mesh section Click Done
4.
This will make the curves visible and hide the elements, so the curves can be picked to create the nodal temperatures. (The curves don’t have to visible to pick them, but for this example it will aid in the selection) Model, Load, Nodal Menu
Creating the Thermal Boundary Conditions
5.
In Entity Selection – Enter Node(s) to Select dialog box
6.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
20-5
Choose the curve that makes up the lower right hand portion of the hole (curve 10)
Curve 9
Curve 10
7.
Click OK
8.
In Create Loads on Nodes dialog box
Highlight Temperature from the selection list 9.
Enter “200” into the Temperature field
10.
Click OK
In Entity Selection – Enter Node(s) to Select dialog box
11.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
Choose the curve that makes up the upper left hand portion of the hole (curve 9) 12.
Click OK
13.
Enter “250” into the Temperature field
20-6 14.
Thermal Stress Analysis - Mounting Plate
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
15.
Choose the 12 curves that make up the outside perimeter of the plate (curves clockwise from top right: 3, 36, 32, 2, 37, 17, 1, 38, 26, 4, 35, 16)
16
35
3
36
4
32
26
2
38
1
16.
Click OK
17.
Enter “70” into the Temperature field
18.
Click OK, then…
17
Click Cancel What View the model with the elements and applied nodal temperatures visible
How
Step 1.
UI Crtl-Q
Command/Display This will bring up the View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
37
Running the Steady-State Thermal Analysis
20-7
2.
CHECK Element box located in the Mesh section, and Thermal box in the Loads section, then…
3.
UNCHECK Curves box located in the Geometry section Click Done
THE THERMAL MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Thermal Analysis” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
20-8 5.
Thermal Stress Analysis - Mounting Plate
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the Plate is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “1..Case 1 Time 1.” from Output Set drop down menu
5.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK
Creating Nodal Temperatures from the Thermal Results
20-9
The contour plot of the temperatures should look like this:
Creating Nodal Temperatures from the Thermal Results The results of the Thermal analysis will used to thermally “load” the plate for a static analysis which will produce a stress value after the model has been constrained.
What Create the Nodal Temperature on all nodes
How
Step 1.
UI
Command/Display Model, Load, From Output
Menu
2.
In Load Set Options for Dynamic Analysis dialog box:
Choose Temperature radio button in the Nodal Loads section
20-10
Thermal Stress Analysis - Mounting Plate
3.
Click OK
4.
In Create Loads From Output dialog box:
Select “1..Case 1 Time 1” from Output Set drop down menu
Select “31..Temperature” from X Vector drop down menu Click OK, then…
5.
In the “OK to Update Existing Temperatures” message window:
Click Yes button Creating the Constraints
What Create pinned nodal constraints
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating Nodal Temperatures from the Thermal Results
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Pinned” in the Title field Click OK
4.
20-11
Model, Constraint, Nodal Menu
5.
In Entity Selection – Enter Node(s) to Select dialog box
6.
Click Method button and highlight On Curve Entity Selection – Enter Node(s) to Select (On Curves)
Choose the 12 curves that make up the outside perimeter of the plate (curves clockwise from top right: 3, 36, 32, 2, 37, 17, 1, 38, 26, 4, 35, 16)
Notice: Because the same exact curves are being picked for this step as where chosen the last time the Entity Selection dialog box was used, the Previous button can be clicked and the curves will be selected again.
16
35
3
36
4
32
26
2
38
1
17
37
20-12 7.
Thermal Stress Analysis - Mounting Plate
Click OK
In the Create Nodal Constraints/DOF dialog box:
Click Pinned button, then…
Click OK, then...
In Entity Selection – Enter Node(s) to Select dialog box
Click Cancel What View the model with the elements and constraints visible
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
CHECK Constraint box located in the Others section, then…
3.
UNCHECK Thermal box in the Loads section Click Done
THE THERMAL STRESS MODEL IS NOW READY TO BE ANALYZED!
Running the Thermal Stress Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
Post-Processing the Thermal Results
1.
20-13
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Thermal Stress” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “1..Static” from the Analysis Type drop down menu
5.
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Static Analysis has created stress results. The best way to view the stress of the Plate is with a contour plot.
What View the stress results in a FEMAP contour plot
How
Step
UI
Command/Display
20-14 1.
Thermal Stress Analysis - Mounting Plate
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Contour radio button in Contour Style section (if not already chosen) Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box: Select “2.. NASTRAN Case 1” from Output Set drop down menu
You will see this box:
5.
, Click OK
Select “7033..Plate Top VonMises Stress” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK The contour plot of the stress should look like this:
This Concludes the Thermal Stress Analysis example. It is recommended to save the model file.
Steady - State Thermal Analysis Circuit Board 21.
A circuit board will be subject to a heat generation loads being created by different sized chips on the board. The temperature of the back side of the plate is 45º C and the ambient temperature of the system is 25º C. The “board” is made of a composite material, and the chips are made of a material with a higher conductivity. A temperature will be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. This model will be used to demonstrate other Heat Transfer capabilities for the next few examples.
Circuit Board
For this example we will be using a model of a circuit board that has already been created including the materials and properties. The analysis process includes:
· creating an ambient temperature body load, as well as, heat generation loads and nodal temperatures.
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements using the section cut and multiple dynamic cutting plane post-processing features of FEMAP.
Importing the Model What
21-2
Steady - State Thermal Analysis - Circuit Board
Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Heat_Transfer/HTBoard.neu Locate HTBoard.neu
Click Open
Neutral File Read Options dialog box:
Click OK
Examining the Material Properties for Thermal Analysis
What Look at the existing material properties in the model
Importing the Model
21-3
How
Step 1.
UI
Command/Display Modify, Edit, Material
Menu
2.
In Entity Selection – Select Material(s) to Edit dialog box: Click Select All button, then…
Click OK
Notice: This step is here to take a look at the values that should be entered at a minimum for any thermal analysis. Please, DO NOT CHANGE THE VALUES or the results of the analysis will be altered and not match those in the example. Also, instead of using the Modify, Edit, Material command, the List, Model, Material command can be used to view the values in the message box located below the main graphics window.
The values of the material are in the following units:
Conductivity, K = W/cmº C Specific Heat, Cp = kJ/kgº C Density (rho) = kg/cm3
21-4 3.
Steady - State Thermal Analysis - Circuit Board
In the Define Material - ISOTROPIC dialog box:
Click OK, then…
View the values for the “Chips” material, then…
Click OK
Creating the Heat Generation Loads and Thermal Boundary Conditions Each “chip” will generate a different amount of heat. The heat generation loads will be placed at the center node of each chip to create an even distribution through the chip The model needs to have an ambient temperature set with a body load and nodal temperatures on the backside of the board. What Creating the Temperature Body Load How Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Heat Generation” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “25” into the Default Temperature (T) field
Creating the Heat Generation Loads and Thermal Boundary Conditions
7.
Click OK
What Creating the Heat Generation loads at the center of each “chip” How Step 1.
UI
Command/Display Model, Load, Nodal
Menu
2.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 378 at center of the large chip
Node 378
Node 434
Node 408
21-5
21-6
Steady - State Thermal Analysis - Circuit Board
3.
Click OK
4.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 5.
Enter “0.12” into the Generation field (The units are in watts)
6.
Click OK
7.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 434 at center of the taller small chip 8.
Click OK
9.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 10.
Enter “0.10” into the Generation field (The units are in watts)
11.
Click OK
12.
Entity Selection – Enter Node(s) to Select dialog box
Select Node 408 at center of the shorter small chip 13.
Click OK
14.
In Create Loads on Nodes dialog box
Highlight Heat Generation from the selection list 15.
Enter “0.08” into the Generation field (The units are in watts)
16.
Click OK, then…
Click Cancel What
Creating the nodal temperatures on the backside of the circuit board
Creating the Heat Generation Loads and Thermal Boundary Conditions
21-7
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click ZX Front button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
3.
Model, Load, Nodal Menu
4.
Entity Selection – Enter Node(s) to Select dialog box
Select Nodes on the backside of the circuit board by holding down the shift key, clicking and dragging the mouse to create a box select around the nodes
Box Selection 5.
Click OK
21-8 6.
Steady - State Thermal Analysis - Circuit Board
In Create Loads on Nodes dialog box
Highlight Temperature from the selection list 7.
Enter “45” into the Temperature field (Units are in º C)
8.
Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Circuit Board” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
Post-Processing the Thermal Results
5.
21-9
Click OK
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the circuit board is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK View, Select or…
3. Menu
4.
Press the F5 Key or choose the view select icon In View Select dialog box:
5.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
6.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “1..Case 1 Time 1.” from Output Set drop down menu
Select “31..Temperature” from Contour drop down menu located in Output Vectors section
21-10 7.
Steady - State Thermal Analysis - Circuit Board
Click OK
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Viewing the internal temperature results can be useful. This can be accomplished by using an Advanced FEMAP Post-Processing feature called Dynamic Cutting Plane which creates a cross-section view of solid element results.
What Utilize FEMAP’s Dynamic Cutting Plane Feature
How
Step 1.
UI Menu
Command/Display View, Advanced Post, Dynamic Cutting Plane
Post-Processing the Thermal Results
2.
21-11
In Dynamic Section Cut Control dialog box:
There is a “slider bar” that can be moved right or left to move the selected cutting plane through the model. The cutting plane can be specified using the Plane button in the dialog box.
Click Plane button
3.
In Plane Locate – Define Primary Cutting Plane dialog box:
4.
Click Method button and highlight Global Plane In Global Plane – Define Primary Cutting Plane dialog box:
5.
Choose YZ Plane radio button Click OK, then…
Move the slider bar back and forth and the model will be cut away as it moves. Stop the bar when the number in the Value field is near 2.5 The Plot should appear something like this:
6.
In Dynamic Section Cut Control dialog box:
Click OK
What
21-12
Steady - State Thermal Analysis - Circuit Board
Create Multiple Cutting Planes for use with FEMAP’s Dynamic Cutting Plane Feature
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Section Cut radio button in Contour Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
5.
Choose Multiple Sections radio button in Section Cut Options section CHECK Section boxes 2 and 3 located in the Section Cut Options section
6.
Click Section 2 Button
7.
In Global Plane – Define Primary Cutting Plane dialog box:
8.
Choose ZX Plane radio button Click OK, then
In Selecting PostProcessing Data dialog box:
9.
Click Section 3 Button In Global Plane – Define Primary Cutting Plane dialog box:
10.
Choose XY Plane radio button Click OK, then…
In Selecting PostProcessing Data dialog box:
Click OK, then…
In View Select dialog box:
Click OK
Post-Processing the Thermal Results
11.
21-13
View, Advanced Post, Dynamic Cutting Plane Menu
12.
In Dynamic Section Cut Control dialog box:
The 1,2,and 3 Section radio buttons are now available for picking
Click the different radio buttons to be able to move the corresponding section planes through the model
Try this: Take Section 1 to a value near 1.5, Section 2 near 2.6, and Section 3 near.175 The Plot should resemble this:
13.
In Dynamic Section Cut Control dialog box:
Click OK
This Concludes the Circuit Board Heat Generation Analysis example. Please save the model file as HTBoard.mod for use in later examples such as Free Convection.
21-14
Steady - State Thermal Analysis - Circuit Board
Steady - State Thermal Analysis Free Convection 22.
The same circuit board will be subject to the same loading conditions as in the last example, but this time Free Convection will be used to allow heat to transfer between the top of the board and the surroundings. By taking Free Convection into account, the temperature will again be calculated at each node in the model using the Steady-State Heat Transfer capability of NX Nastran. The temperatures on the circuit board based on the Conduction only conditions that existed in the last example are worst case because heat was not able to transfer to the surroundings using Free Convection.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating a Free Convection thermal condition on the top surface of the circuit board
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements and the contour plot of the Convection Surface using groups
Opening an Existing FEMAP Model What Open an existing FEMAP model file HTBoard.mod.
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Heat_Transfer/HTBoard.mod
Click Open
22-2
Steady - State Thermal Analysis - Free Convection
If the circuit board model is showing any contours or section cuts, Press the F5 button on the keyboard, then choose the None – Model Only radio button in the Contour Style section and Click OK.
The model should only be showing elements and thermal loads to begin the example.
Creating the Free Convection Boundary Conditions The top surface of the circuit board will allow Free Convection to the surroundings. It is required to have a convection heat transfer coefficient (h) in order to create the proper effects due to free convection. For this example we will use h = 4.1 x 105 W/mm2 º C.
What Create the Free Convection Boundary Condition
How
Step 1.
UI
Command/Display Model, Load, Elemental
Menu
2.
Entity Selection – Enter Elements(s) to Select dialog box
Click Select All button, then…
Click OK
Creating the Free Convection Boundary Conditions
3.
22-3
In Create Loads on Elements dialog box
Highlight Convection from the selection list 4.
Enter “4.1E-5” into the Coefficient field, then…
5.
Enter “25” in the Temperature field Click OK
6.
In Face Selection for Elemental Loads dialog box:
7.
Choose Adjacent Faces radio button in Method section, then… Click in Face field to activate
Select the top Element face of ANY Element on the top surface of the circuit board (not the chips)…for example face 2 on Element 82
Element 82
22-4 8.
Steady - State Thermal Analysis - Free Convection
Click OK, then…
Click Cancel
Notice: Creating this type of convection condition will actually create plot-only planer elements on the model and FEMAP will require the model be saved during the Analyze step for proper post-processing.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Use an existing analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
Post-Processing the Thermal Results
2.
22-5
In Analysis Set Manager dialog box:
Click Analyze button
Notice: An analysis should already exist in HTBoard.mod. If one does not, please follow the Running the Steady-State Thermal Analysis section from Example 21.
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the circuit board is with a contour plot. The Elemental Free Convection values can also be viewed with a contour plot of a selected group.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
3.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
22-6
Steady - State Thermal Analysis - Free Convection
4.
In View Quick Options dialog box:
5.
Click All Entities Off button CHECK Element box located in the Mesh section
6.
Click Done
7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
9.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Notice the Maximum Nodal Temperature is lower due to the effects of free convection
Post-Processing the Thermal Results
22-7
What View the temperature results in a FEMAP animation
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Animate radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
Select “31..Temperature” from Deformation and Contour drop down menus located in Output Vectors section
5.
Notice: FEMAP needs a deformation vector to animate a contour plot, therefore use Temperature as the deformation vector. The Temperature will not actually be used deform the model, but a deformation vector does need to be selected. Click OK
6.
In View Select dialog box:
7.
CHECK Skip Deformation box Click OK
The speed of the animation can be controlled by using the View, Advanced Post, Animation command while the Model is animating. Click the Slower and Faster buttons until the desired viewing speed has been found
Creating a Group for viewing purposes
What Create a group containing an element type in order to view contours on the Convection Surface only.
How
22-8
Step 1.
UI
Steady - State Thermal Analysis - Free Convection
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Convection Surface” in the Title field Click OK
4.
Group, Element, Type Menu
5.
In Entity Selection – Select Element Types for Group dialog box:
Select “32..L Plot Planar” from Type drop down menu
Notice: Remember that FEMAP created these Plot-planer elements to be used with the Convection “loading” condition Click OK
6. 7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
on the View Toolbar
9.
Choose None - Model Only radio button in Deformed Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “80031..Elem Free Convection” from Contour drop down menu located in Output Vectors section Click OK, then…
In View Select dialog box:
Click Model Data button
Post-Processing the Thermal Results
12.
In Select Model Data for View dialog box:
13.
Choose Active radio button Group section Click OK, then…
22-9
In View Select dialog box:
Click OK The Plot of the Free Convection values should look like this:
This Concludes the Circuit Board Free Convection example. Please save the model file as HTFree.mod.
22-10
Steady - State Thermal Analysis - Free Convection
Temperature - Dependent effects Circuit Board 23.
The same circuit board will be subject to the same loading conditions as in the last two examples, but this time the conductivity of the Material Property of the chips will be temperature dependent, as well as, the Convection Coefficient.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating functions to represent temperature-dependence for the Conductivity of the Chips and for the Free Convection Coefficient
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing the contour plot of the solid elements and the contour plot.
Opening an Existing FEMAP Model What Open an existing FEMAP model file HTBoard.mod.
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Open Menu
3.
Read Model from Open dialog box:
Locate: FEMAP93/Examples/Heat_Transfer/Temperature Dependent Circuit/HTBoard.mod
Click Open
23-2
Temperature - Dependent effects - Circuit Board
Use the View, Select command. Choose None-Model Only for both Contour Style and Deformed Style. Then Click OK.
Creating a Temperature Dependent Material Property A function will be created to define the relationship between Temperature and Conductivity for the “Chips” Material Property. This function will then be referenced by the Material Property using a portion of the Define Material dialog box.
What Create Conductivity vs. Temperature (k vs. T) function How
Step 1.
UI
Command/Display Model, Function
Menu
2.
Tip: You can also create a new Function using the New command on the “context sensitive menu” located on the Functions branch in the Model Info tree (simply click to highlight the top level of the Functions branch or any existing Function, then right mouse click to see the context sensitive menu). In Function Definition dialog box:
3.
Type “Chips (k vs. T)” in the Title field Select “2..vs. Temperature” from Type drop down menu.
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 10, Y = 0.333, Then…Click More button X = 30, Y = 0.386, Then…Click More button X = 50, Y = 0.415, Then…Click More button X = 70, Y = 0.437, Then…Click More button X = 90, Y = 0.452, Then…Click More button X = 120, Y = 0.461, Then…Click More button X = 200, Y = 0.461
Creating a Temperature Dependent Material Property
6.
23-3
Click OK, then
Click Cancel
What View Conductivity vs. Temperature (k vs. T) function using FEMAP’s XY Plot Capabilities How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
on the View Toolbar
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..Chips (k vs. T)” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key)
23-4
Temperature - Dependent effects - Circuit Board
The XY Plot should look like this:
What Modify the Chips Material Property to reference the k vs. T function
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Quick Hidden Line radio button Click OK button
4.
Modify, Edit, Material Menu
5.
Entity Selection – Select Material(s) to Edit dialog box:
Select any element on one of the “Chips”
on the View Toolbar
Creating a Temperature Dependent Convection Coefficient (h)
6.
23-5
Click OK, then…
Tip: You can also edit an existing Material using the Edit command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight any existing Material, then right mouse click to see the context sensitive menu). In this case, you would highlight “1..Chips” in the list in the Materials branch, then right click and choose Edit. In the Define Material - ISOTROPIC dialog box:
7.
Click the Function References tab
Notice: The Message at the top of the Function References portion of the dialog box, “Press CtrlF in each field to select from a list of the available functions”, explains an easy way to choose the desired function for all fields that will have function-dependence. Be sure to have the proper field reference the correct function.
8.
Ctrl-F
Click in the Conductivity, K field, making it active In Select Function dialog box:
9.
Highlight 1..Chips (k vs. T) from the selection list Click OK
10.
In the Define Material - ISOTROPIC dialog box:
Click the General tab
11.
Click in the Conductivity, K field, making it active Enter “1.0” in the Conductivity, k field (1.0 * function value)
12.
Click OK
Creating a Temperature Dependent Convection Coefficient (h) A function will be created to define the relationship between Temperature and Free Convection Coefficient. This function will then be referenced by the Convection “loads”.
What Create Convection Coefficient vs. Temperature (h vs. T) function
23-6
Temperature - Dependent effects - Circuit Board
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Convection Coeff” in the Title field Select “2..vs. Temperature” from Type drop down menu.
4.
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 10, Y = 1.2E-5, Then…Click More button X = 30, Y =5.3E-5, Then…Click More button X = 50, Y = 8.9E-5, Then…Click More button X = 70, Y = 1.2E-4, Then…Click More button X = 90, Y = 3.1E-4, Then…Click More button X = 120, Y = 5.1E-4, Then…Click More button X = 200, Y = 5.1E-4 Click OK, then…
6.
Click Cancel
What Create the Free Convection Boundary Condition
How
Step 1.
UI Menu
Command/Display Model, Load, Elemental
Creating a Temperature Dependent Convection Coefficient (h)
2.
23-7
Entity Selection – Enter Element(s) to Select dialog box
Click Select All button, then…
3.
Click OK In Create Loads on Elements dialog box
Highlight Convection from the selection list 4.
Enter “1.0” into the Coefficient field, then…
5.
Enter “25” in the Temperature field Select “2..Convection Coeff” from Time/Freq Dependence drop down menu located next to the Coefficient field
6.
Click OK
7.
In Face Selection for Elemental Loads dialog box:
8.
Choose Adjacent Faces radio button in Method section, then… Click in Face field to activate
Select the top Element face of ANY Element on the top surface of the circuit board (not the chips)…for example face 2 on Element 82
Element 82
23-8
9.
Temperature - Dependent effects - Circuit Board
Click OK, then…
Click Cancel
Notice: Creating this type of convection condition will actually create plot-only planer elements on the model and FEMAP will require the model be saved during the Analyze step for proper post-processing.
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
Post-Processing the Thermal Results
23-9
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
Click Analyze button
Notice: An analysis should already exist in HTBoard.mod. If one does not, please follow the Running the Steady-State Thermal Analysis section from Example 21.
Post-Processing the Thermal Results The Steady-State Heat Transfer Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution based on the Temperature Dependency across the circuit board is with a contour plot.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Rotate, Model or…
Menu
Press the F8 Key 2.
In View Rotate dialog box:
Click Dimetric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
23-10 3.
Crtl-Q
Temperature - Dependent effects - Circuit Board
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 4.
In View Quick Options dialog box:
5.
Click All Entities Off button CHECK Element box located in the Mesh section
6.
Click Done
7.
View, Select or… Menu
8.
Press the F5 Key or choose the view select icon In View Select dialog box:
9.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
10.
In Selecting PostProcessing Data dialog box:
on the View Toolbar
Select “2..Case 1 Time 1.” from Output Set drop down menu
11.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK, then...
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Post-Processing the Thermal Results
23-11
The Maximum temperature is lower than the two previous examples due to the representing the Material properties and Convection Coefficient with a higher degree of accuracy and realism.
Using the Dynamic Isosurface Feature of FEMAP
The Dynamic Isosurface is utilized to show areas of identical results values throughout a model containing solid elements. In this case, the results values of interest are temperatures and this feature will always use the selected Contour Output Vector to create the isosurfaces.
What
Utilize the Dynamic IsoSurface feature of FEMAP How
Step 1.
UI
Command/Display View, Advanced Post, Dynamic IsoSurface
Menu
2.
In Dynamic IsoSurface Control dialog box:
There is a “slider bar” that can be moved right or left to move the isosurface through the model to view the areas of identical value
3.
Move the bar through the entire rang of values (from left to right). After seeing the entire range of values, try moving the slider bar until the value reaches just above 45, 60, 75, and 95 to examine the different isosurface at each value. Then… Click OK
The model should be contoured fully again.
This Concludes the Circuit Board with Temperature Dependent Factors Analysis example. Please save the model file as HTTDBoard.mod.
23-12
Temperature - Dependent effects - Circuit Board
24.
Enclosure Radiation
Three plates will be used for this simple example of Enclosure Radiation. The plates on each side “Can be shaded” and the center plate “Can shade” the other two. An Emissivity Value will be assigned to each “face” of the plates that will be involved in the analysis. The geometry will be created using FEMAP.
For this example we will be using a model of a circuit board that has already been created. The analysis process includes:
· creating geometry to represent the plates, then meshing the model with parabolic elements
· assigning Emissivity values and applying heat flux to the model
· analyzing the model with NX Nastran’s Steady-State Heat Transfer Solution Method
· viewing contour plots of the nodal temperature results
Opening a FEMAP Model What Open a new FEMAP model file.
How
Step 1.
UI
Command/Display File, New
Menu
Creating the Geometry
Three surfaces must be created for this model.
What Create the surfaces
24-2
Enclosure Radiation
How
Step 1.
UI
Command/Display Geometry, Surface, Corners
Menu
2.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = 0, Then…Click OK button X = 5, Y = 0, Z = 0, Then…Click OK button X = 5, Y = 5, Z = 0, Then…Click OK button X = 0, Y = 5, Z = 0, Then…Click OK button 3.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = 4, Then…Click OK button X = 5, Y = 0, Z = 4, Then…Click OK button X = 5, Y = 5, Z = 4, Then…Click OK button X = 0, Y = 5, Z = 4, Then…Click OK button 4.
Enter these values into the corresponding fields:
X = 0, Y = 0, Z = -3, Then…Click OK button X = 5, Y = 0, Z = -3, Then…Click OK button X = 5, Y = 5, Z = -3, Then…Click OK button X = 0, Y = 5, Z = -3, 5.
Click OK, then
Click Cancel
Creating Materials and Properties
Creating Materials and Properties
What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
In Define Material - ISOTROPIC dialog box:
Type “Plates” in Title field, then…
Enter “237” in Conductivity, k field (units: W/m º K)
Enter “903” in Specific Heat, Cp field (units: J/kg º K)
Enter “2702” in Mass Density field (units: kg/m3) Click OK, then…
3.
Click Cancel
What Create a Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – PLATE Element Type dialog box:
Type “Plates” in Title field, then…
3.
Enter “0.001” in Thicknesses, Tavg or T1 field Select “Plates” from the Material drop down menu
24-3
24-4
Enclosure Radiation
4.
Click Elem/Property button
5.
In Element / Property Type dialog box:
CHECK Parabolic Elements at the top of the dialog box
Notice: This will create second order elements (parabolic) with mid-side nodes when the plates are meshed. Click OK, then…
6.
In Define Property – PLATE Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Plates
What Set the mesh size
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Default Size
Menu
2.
In Default Mesh Size dialog box:
3.
Enter “1” in both the Size and Min Elem fields, Click OK
What Mesh the plates
How
Step
UI
Command/Display
Creating Materials and Properties
1.
24-5
Mesh, Geometry, Surface Menu
2.
In Entity Selection – Select Surfaces to Mesh dialog box:
Click Select All button, then…
3.
Click OK In Automesh Surfaces dialog box:
4.
Select “Plates” from the Property drop down menu CHECK Midside Nodes on Geometry box
5.
Click OK
6.
View, Rotate, Model or… Menu
Press the F8 Key 7.
In View Rotate dialog box:
Click Isometric button, then…
Click OK Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
8.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 9.
In View Quick Options dialog box:
Click All Entities Off button, then
10.
Click Loads/Constraints On button CHECK Element box located in the Mesh section
24-6 11.
Enclosure Radiation
Click Done
The model should now look like this:
Reversing the Element Normals The plate elements have two “faces” each. Because the model is representing an enclosure, the normals of the elements on the two outer surfaces must point towards the middle surface. First the element normals need to be turned on in order to see which elements are not pointing towards the center. Next the elements with normals not facing the middle plate will be modified.
What View the Element Normals
How
Step 1.
UI
Command/Display View, Options or…
Menu
2.
3.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose Labels, Entities and Color radio button under Category Highlight “Element - Directions” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “1..Normal Vectors” from the Normal Style selection list
Reversing the Element Normals
4.
CHECK Show Direction box in upper right corner of dialog box
5.
Click OK
The normal vector should now be visible:
Element Normals need to be reversed on left plate
The normal vectors need to be reversed on the left plate while in Isometric View (shown) What Reverse the element normals
How
24-7
24-8
Step 1.
UI
Enclosure Radiation
Command/Display Modify, Update Elements, Reverse Normal/Orient First Edge
Menu
2.
In Entity Selection – Select Element(s) to Update Direction dialog box:
3.
Click Method button and highlight On Surface Entity Selection – Select Element(s) to Update Direction (On Surfaces)
Choose the surface on the left side of the graphics window (Surface 2) 4.
Click OK
5.
In Update Element Directions dialog box:
Choose Reverse Element Direction radio button
6. 7.
Click OK Ctrl-G
Window, Regenerate (This will Regenerate the model in order to see the changes)
The Model should now look like this:
Creating Radiation Emissivity and Heat Flux Loads
24-9
Creating Radiation Emissivity and Heat Flux Loads Because the middle surface will need to radiate to both other surfaces an Emissivity value needs to be placed on both “faces” of the middle surfaces elements. The Emissivity values are created by “loading the face” of the elements and defining whether the elements “Can Shade” or “Can be Shaded” after the selection of the Enclosure Radiation option.
What Create a load set and Body Load
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Radiation” in the Title field Click OK
4.
Model, Load, Body Menu
5.
In Create Body Loads dialog box:
6.
CHECK active box for Default Temperature (T) field to become available Enter “475” into the Default Temperature (T) field
7.
Click OK
What Create Radiation settings
How
Step 1.
UI Menu
Command/Display Model, Load, Heat Transfer
24-10 2.
Enclosure Radiation
In Heat Transfer Loads dialog box:
Enter “5.670E-8” in the Stefan-Boltzmann field (units: W/m2º K4)
3.
Click OK
What Create Radiation “loads”
How
Step 1.
UI
Command/Display Model, Load, Elemental
Menu
2.
In Entity Selection – Enter Elements(s) to Select dialog box
3.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the left hand surface (Surface 2) 4.
Click OK
Creating Radiation Emissivity and Heat Flux Loads
5.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 6.
CHECK Enclosure Radiation box, then… Can Be Shaded box
7.
Enter “1.0” into the Emissivity field
8.
Click OK
9.
In Face Selection for Elemental Loads dialog box
Enter “1” into the Face field
24-11
24-12 10.
Enclosure Radiation
Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
11.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the right hand surface (Surface 3) 12.
Click OK
13.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 14.
CHECK Enclosure Radiation box, then… Can Be Shaded box
15.
Enter “1.0” into the Emissivity field
16.
Click OK
17.
In Face Selection for Elemental Loads dialog box
18.
Enter “1” into the Face field Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
19.
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
Choose the surface on the middle surface (Surface 1) 20.
Click OK
21.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 22.
CHECK Enclosure Radiation box, then… Can Shade box
23.
Enter “1.0” into the Emissivity field
24.
Click OK
Creating Radiation Emissivity and Heat Flux Loads
25.
In Face Selection for Elemental Loads dialog box
26.
Enter “1” into the Face field Click OK
In Entity Selection – Enter Elements(s) to Select dialog box
Click Method button and highlight On Surface Entity Selection – Enter Element(s) to Select (On Surface)
27.
Choose the surface on the middle surface (Surface 1) 28.
Click OK
29.
In Create Loads on Elements dialog box
Highlight Radiation from the selection list 30.
CHECK Enclosure Radiation box, then… Can Shade box
31.
Enter “1.0” into the Emissivity field
32.
Click OK
33.
In Face Selection for Elemental Loads dialog box
34.
Enter “2” into the Face field Click OK, then…
Click Cancel What Create Heat Flux Load on element
How
Step 1.
UI Menu
Command/Display Model, Load, Elemental
24-13
24-14 2.
Enclosure Radiation
Entity Selection – Enter Element(s) to Select
Choose the center element on the middle surface (Element 13)
Element 13
3.
Click OK
4.
In Create Loads on Elements dialog box
Highlight Heat Flux from the selection list 5.
Enter “1200” into the Flux field
6.
Click OK
7.
In Face Selection for Elemental Loads dialog box
8.
Enter “1” into the Face field Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Steady-State Thermal Analysis What Create an analysis case for Steady-State Heat Transfer using the FEMAP Analysis Set Manager
How
Post-Processing the Thermal Results
Step 1.
UI
24-15
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Radiation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “20..Steady-State Heat Transfer” from the Analysis Type drop down menu
5.
Click Next 7 times
6
In Boundary Conditions dialog box:
7.
Select “1..Radiation” from Load AND Initial Conditions drop down menus Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Post-Processing the Thermal Results The Radiation Analysis has created a resultant nodal temperature at each node. The best way to view the temperature distribution across the Plate is with a contour plot.
What
24-16
Enclosure Radiation
Create a group
How
Step 1.
UI
Command/Display Group, Set
Menu
2.
In Create or Activate Group dialog box:
3.
Type “Parabolic Elements” in the Title field Click OK
4.
Group, Element, Type Menu
5.
In Entity Selection – Select Element Types for Group dialog box:
Select “18..P Plate” from Type drop down menu
Notice: This will allow better viewing of the plate element results Click OK
6.
What View the temperature results in a FEMAP contour plot
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
on the View Toolbar
Post-Processing the Thermal Results
4.
24-17
In Selecting PostProcessing Data dialog box:
Select “1..Case 1 Time 1.” from Output Set drop down menu
5.
Select “31..Temperature” from Contour drop down menu located in Output Vectors section Click OK, then…
In View Select dialog box:
6.
Click Model Data button In Select Model Data for View dialog box:
7.
Choose Active radio button Group section Click OK, then…
In View Select dialog box:
Click OK The contour plot of the temperatures should look like this:
Notice that the plate further away from the middle plate has a lower temperature.
This Concludes the Enclosure Radiation example. Please save the model file as Radiation.mod.
24-18
Enclosure Radiation
Plastic Deformation of Rod Nonlinear Material 25.
A simple rod model will be built out of a material which will become nonlinear after the model reaches a defined yield criteria (von Mises Stress). The model will be loaded axially beyond the yield stress and then unloaded. These loading conditions will leave the rod plastically deformed. The displacement and strain results will then be viewed with an XY plot.
For this example a model made of rod elements will be created using FEMAP. The analysis process includes:
· creating a function to represent a strain vs. stress curve and use it to define a nonlinear material
· creating the mesh, loads, and boundary conditions
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the displacements and strains using FEMAP’s XY Plotting Capabilities
Open a New FEMAP Model File
Creating the Nonlinear Material What Create a simple stress vs. strain function
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Strain vs. Stress” in the Title field Select “4..vs. Stress” from Type drop down menu.
25-2
Plastic Deformation of Rod - Nonlinear Material
4
Choose Single Value radio button
5.
Enter these values into the corresponding fields:
X = 0, Y = 0, Then…Click More button X = 180, Y = 0.001, Then…Click More button X = 235, Y = 0.003, Then…Click More button X = 270, Y = 0.005 Click OK, then...
6.
Click Cancel Visual verification of the Strain vs. Stress curve (or any function) is always a good idea.
What Verify the Stress vs. Strain curve using the XY Plotting Feature of FEMAP
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose XY of Function radio button Click Model Data button
4.
In Select Model Data for View dialog box:
5.
Select “1..Strain vs. Stress” from Select drop down menu located in the Function portion of the window Click OK
In View Select dialog box:
Click OK
from the View Toolbar
Creating the Nonlinear Material
25-3
Tip: There is quick method to bring up a special view called “XY Show” in the FEMAP user interface, specifically to view a single XY plot of functions (up to 9 can be shown at once). This is accomplished using the Functions branch of the Model Info tree (Functions can be found in the Model branch). Expand the Functions branch and all functions currently in the model will be listed. To bring up this view, you need to use the Show command on the “context sensitive menu” for Functions. Simply highlight up to 9 functions, then right-mouse click and choose the Show command. A new view called “XY Show” will appear in FEMAP and can be closed at any time, but will the view will remain in the model. If you want to remove the “XY Show” view permanently, you must delete it using the Delete, View... command or highlighting “XY Show” in the View branch of the Model Info tree and pressing the Delete key. You can change the colors and other parameters of each curve using the “XY Curve #” options in the PostProcessing category of View, Options (F6 key) View, Options or…
6. Menu
7.
8.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “XY Curve 1” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “2..Output Values” from Data Labels selection list
Highlight “Lines with Points” from Curve Style selection list
25-4 9.
Plastic Deformation of Rod - Nonlinear Material
Click OK
The Stress vs. Strain Curve should look like this:
What Create the Material
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Draw Model radio button Click OK
4.
Model, Material Menu
from the View Toolbar
Creating the Property and Mesh
5.
25-5
In Define Material - ISOTROPIC dialog box:
Type “Nonlinear Material” in Title field, then…
Enter “200,000” in Young’s Modulus, E field (units: N/mm2)
6.
Enter “0.3” in Poisson’s Ratio, nu field Click Nonlinear tab
7.
In the Nonlinear portion of the Define Material - ISOTROPIC dialog box:
8.
Choose Plastic radio button Select “1..Strain vs. Stress” from Time/Freq Dependence drop down menu located in the Nonlinear Properties section
9.
Select “0..von Mises” from the Yield Criterion drop down menu in the Yield Function section Enter “180” in Initial Yield Stress field
10.
Click General tab of the Define Material - ISOTROPIC dialog box
11.
Click OK, then…
Click Cancel
Creating the Property and Mesh What Create a Property
How
Step 1.
UI Menu
Command/Display Model, Property
25-6
Plastic Deformation of Rod - Nonlinear Material
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Rod radio button in Line Elements section Click OK
5.
In Define Property – ROD Element Type dialog box:
Type “Rod” in Title field
6.
Enter “1” in Area, A field Select “Nonlinear Material” from Material drop down menu
7.
Click OK, then…
Click Cancel What Create the Nodes and Elements
How
Step 1.
UI
Command/Display Mesh, Between
Menu
2.
In Generate Between Corners dialog box:
3.
Select “Rod” from the Property drop down menu Enter “11” in #Nodes field
4.
Click OK
Creating Loads and Constraints
5.
25-7
In the Locate – Enter Corner 1 of Mesh (Cancel to Abort or Backup) dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 100, Y = 0, Z = 0 Click OK
6.
Creating Loads and Constraints Two Load Sets must be created in order to simulate a loading condition and an “unloaded” condition. A load does need to be applied for the unloaded condition for the analysis to run, so a very small load will be applied axially in a second load set to accomplish the “relaxation” of the rod.
What Create the fixed constraint
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the node at the left side end of the rod (Nodes 1)
25-8 6.
Plastic Deformation of Rod - Nonlinear Material
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
7.
Click OK, then… In Entity Selection – Enter Node(s) to Select dialog box:
8.
Click Cancel View, Autoscale, Visible Menu
OR Press Ctrl - A What Creating the “Loading” Load Set
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Loaded” in the Title field Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the rod (Nodes 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list
Creating Loads and Constraints
8.
Enter “300” in FX field (units: N)
9.
Click OK, then…
Click Cancel What Creating the “Unloading” Load Set
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
Enter “2” in ID field
Type “Unloaded” in the Title field Click OK
3. 4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the rod (Nodes 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “0.001” in FX field (units: N)
9.
Click OK, then…
Click Cancel
What Create Nonlinear Static settings (They must be set for BOTH Load Sets)
25-9
25-10
Plastic Deformation of Rod - Nonlinear Material
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
Running the Nonlinear Static Analysis with two cases
7.
25-11
Model, Load, Set Menu
8.
In Create or Activate Load Set dialog box:
Highlight “1..Loaded” from the list 9.
Click OK
10.
Model, Load, Nonlinear Analysis Menu
11.
In Load Set Options for Nonlinear Analysis dialog box:
12.
Choose Static radio button Click Copy button
13.
Notice: This will copy the values of this dialog box that have been entered in another selected Load Set into the Active Load Set In Create or Activate Load Set dialog box:
Highlight “2..Unloaded” from the list 14.
Click OK, then…
In Load Set Options for Nonlinear Analysis dialog box:
Click OK THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis with two cases What Create an analysis set with multiple cases for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
25-12 1.
Plastic Deformation of Rod - Nonlinear Material
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Plastic Deformation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next 7 times
6.
In Nastran Output Requests dialog box:
7.
CHECK Strain in the Elemental Section Click OK, then…
In Analysis Set Manager dialog box:
Click Multi-Set button
Running the Nonlinear Static Analysis with two cases
8.
25-13
In Entity Selection – Select Constraint Set(s) to Generate Cases dialog box:
Click Select All, then…
Click OK
9.
In Entity Selection – Select Load Set(s) to Generate Cases dialog box:
Click Select All, then…
Click OK
10.
In Analysis Set Manager dialog box:
Double Click the words “Analysis Set: 1..Plastic Deformation” or click the “+” sign to the left of them.
The Analysis Set Manager Tree Structure will expand to show the different sections of the load case (Solution Options, Options, Master Control and Requests, Cases)
Two cases have been created: (Case names based on Load and constraint sets) Case: 1..Fixed – Loaded Case: 2..Fixed – Unloaded
Notice: All dialog boxes in the Analysis Set Manager can also be reached through the Tree Structure.
25-14
Plastic Deformation of Rod - Nonlinear Material
New Analysis Cases
11.
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”... Click Yes
Post-Processing the Results A multi-set animation of the results would show the plastic deformation, but due to the relatively small displacements in this model, a XY plot of the displacements and strain values would create a clearer method to visualize this results.
What Create a XY Plot of displacement of a single node of the rod over all the output sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Post-Processing the Results
2.
In View Select dialog box:
3.
Choose XY vs. Set Value radio button Click XY Data button
4.
In Select XY Curve Data dialog box:
25-15
Select “1..Case 1 Time 0.1” from drop down menu located in the Output Set section, then…
5.
Select “1..Total Translation” from drop down menu located in the Output Vector section Enter “11” in the Node field located in the Output Location section
6.
Leave the From and To fields in Show Output Set Section bank to plot the Output Vector over the range of the analysis Click OK, then…
In View Select dialog box:
Click OK The Plot of Node 11’s Total Translation should look like this:
What Create a XY Plot of plastic strain of a single element of the rod over all the output sets
25-16
Plastic Deformation of Rod - Nonlinear Material
How
Step 1.
2.
UI
Command/Display Right click in the Graphics window and choose XY Data from the menu
In Select XY Curve Data dialog box:
Select “1..Case 1 Time 0.1” from drop down menu located in the Output Set section, then…
3.
Select “3286..Rod Plastic Strain” from drop down menu located in the Output Vector section Enter “10” in the Element field located in the Output Location section
4.
Click OK
The Plot of Element 10’s Plastic Strain should look like this:
This Concludes the Large Deformation example. It is recommended to save the model file.
26.
Gap Contact - Cantilever Beam
A cantilever beams with a tubular cross section will be used to demonstrate Gap Contact found in Nonlinear Static Analysis. The beam will have one end fixed, and the free end will be loaded with a Force. During the analysis, the deformation of the model will cause the gap to close creating contact. Contact in analysis almost always signals the use of a nonlinear solution. This example will use the Nonlinear Static solving capability of NX Nastran.
For this example a beam model will be created using FEMAP. The analysis process includes:
· creating a beam property, meshing an existing curve
· creating a Gap property and the gap element, then loads and constraints
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the stresses on the beam using FEMAP’s Beam Diagram post-processing capability
Creating the Geometry What Create lines to represent the beams
How
Step 1.
UI
Command/Display File, New
Menu
2.
Geometry, Curve-Line, Coordinates Menu
26-2 3.
Gap Contact - Cantilever Beam
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 10, Y = 0, Z = 0 Click OK, then…
4.
Click Cancel, then press Ctrl-A to Autoscale the visible parts of the model
Creating the Materials and Properties What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
Tip: You can also create a new Material using the New command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight the top level of the Materials branch or any existing Material, then right mouse click to see the context sensitive menu). In Define Material - ISOTROPIC dialog box:
3.
Click Load In Select From Library dialog box:
Highlight “AISI 4340 Steel” from the selection list
Notice: Any material properties entered manually by the user can be saved in the library and recalled for future use by giving the material a name and clicking the save button in the Define Material - ISOTROPIC dialog box. To place the material in a new model, click the Load button, select it from the list and click OK.
Creating the Materials and Properties
4.
26-3
Click OK, then…
In Define Material - ISOTROPIC dialog box:
Click OK, then…
Click Cancel What Create the tubular Beam Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
Tip: You can also create a new Property using the New command on the “context sensitive menu” located on the Properties branch in the Model Info tree (simply click to highlight the top level of the Properties branch or any existing Property, then right mouse click to see the context sensitive menu). In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Beam radio button in Line Elements section Click OK
5.
In Define Property – BEAM Element Type dialog box:
6.
Type “Square Tube” in Title field Select “AISI 4340 Steel” from the Material drop down menu
7.
Click Shape button
8.
In Cross Section Definition dialog box:
Select “Rectangular Tube” from the Shape drop down menu
26-4 9.
Gap Contact - Cantilever Beam
Enter the following values into the corresponding fields in the Size section of the dialog box:
Height = 0.5
Width = 0.5
Thickness = 0.1
Click the Draw Section Button to see the defined section
10.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Curves
What Set the mesh size on the curves
Creating the Materials and Properties
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Size Along Curve
Menu
2.
Entity Selection – Select Curve(s) to Set Mesh Size
Choose the curve (curve 1) 3.
Click OK
4.
In Mesh Size Along Curves dialog box:
5.
Enter “10” in Number of Elements field Click OK, then…
Click Cancel
What Mesh the line
How Step 1.
UI
Command/Display Mesh, Geometry, Curve
Menu
2.
Entity Selection – Select Curve(s) to Mesh
Choose curve 1 3.
Click OK
4.
In Geometry Mesh Options dialog box:
5.
Select “Square Tube” from the Property drop down menu Click OK
6.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 1, Z = 0
26-5
26-6
Gap Contact - Cantilever Beam
7. 8.
Click OK, then… Crtl-Q
This will bring up the View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 9.
Click Geometry Off button, then…
Click Done
Creating the Gap property and element Every Gap element MUST have a Gap property associated with it that has the correct Initial Gap distance value. Compression and Tension Stiffness values are also required to control the closing of the “gap”. In this example, only one gap element is required, therefore only one Gap Property must be created. If a model would require multiple Gap elements to be created at a number of different initial gap distances, then an individual Gap Property must be created for EVERY different initial gap distance. Gap Contact is a node-to-node method of contact and therefore should have a corresponding number and spacing of nodes on each contact line or surface for effective convergence of the Nonlinear Analysis.
What Create a Node to represent the other side of the “Gap”
How
Step 1.
UI
Command/Display Model, Node
Menu
2.
In the Locate – Enter Coordinates or Select with Curser dialog box:
3.
Enter: X = 7, Y = -0.5, Z = 0, Click OK, then…
Click Cancel
What Create a Gap Property
How
Creating the Gap property and element
Step 1.
UI
26-7
Command/Display Model, Property
Menu
2.
In Define Property – BEAM Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Gap radio button in Line Elements section Click OK
5.
In Define Property – GAP Element Type dialog box:
Type “Gap” in Title field
Enter “0.5” in Initial Gap field
Enter “1000000” in Compression Stiffness field
Enter “0.0001” in Tension Stiffness field
Notice: A great way to determine the Initial Gap value for a gap of undetermined distance is to use the “Distance Measurement Tool” in FEMAP. This can be accessed by highlighting the Initial Gap field (or any other dialog box field which requires a distance) and pressing Ctrl-D on the keyboard. This will bring up a “point-to-point” measuring tool prompting the user to choose a start point, clicking OK, then prompting for an end point and clicking OK. This is a very helpful FEMAP tool.
26-8 6.
Gap Contact - Cantilever Beam
Click OK, then…
Click Cancel What Create a Gap element between a node on the beam and the newly created node
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define GAP Element – Enter Nodes or Select with Cursor dialog box:
Choose the 8th node from the left side of the beam (Node 8) and the newly created node (Node 12)
Node 8
Node 12
3.
Click Vector button
4.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 5.
Tip X = 0, Y = 0, Z = 1 Click OK
6.
In Define GAP Element – Enter Nodes or Select with Cursor dialog box:
Select “Gap” from the Property drop down menu
Creating the loads and constraints
7.
Click OK, then…
Click Cancel
Creating the loads and constraints What Apply a fixed constraint to the left end of the beam and the “bottom node” of the Gap
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
26-9
26-10 5.
Gap Contact - Cantilever Beam
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the fixed end of the beam (Nodes 1) and the node on the “bottom” of the gap (node 12)
Node 1
Node 12
6.
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Apply a Force to the free end of the beam
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Force” in the Title field Click OK
Creating Settings for Nonlinear analysis
4.
26-11
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of the beam (Node 11) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 8.
Enter “-2000” in FY field (units: Pounds)
9.
Click OK, then…
Click Cancel The model should now look like this:
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the
26-12
Gap Contact - Cantilever Beam
steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX Nastran through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
Running the Nonlinear Static Analysis
26-13
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Gap Contact” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
26-14
Gap Contact - Cantilever Beam
Post-Processing the Gap Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation results of the beams is with a deformed plot. The best ways to view the stress results on the beam is with the Beam Diagram contour capability.
What View the results in a FEMAP Beam Diagram plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Beam Diagram radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “10..Case 10 Time 1.” from drop down menu located in the Output Set section, then…
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
5.
Select “3139..Beam EndA Pt1 Comb Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
In View Select dialog box:
Click OK
Post-Processing the Gap Contact Results
6.
26-15
Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting PostProcessing as the Category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Command Toolbar for this task View, Options or…
7. Menu
8.
9.
Press the F6 Key or choose “options” from the view icon In View Options dialog box:
on the View Toolbar
Choose PostProcessing radio button under Category Highlight “Beam Diagram” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “3..Global Y” from the Default Direction selection list
26-16
10.
Gap Contact - Cantilever Beam
Click OK
The Beam Diagram plot of the deformed model should look like this:
This Concludes the Gap Contact example. It is recommended to save the model file.
Large Deformation - Cantilever Beam 27.
Nonlinear Analysis is analysis which often consists of models which undergo large deformations due to geometric or material nonlinearities. This realm of analysis includes such other concepts as plastic deformation, snap-through, creep, physical contact between objects, shrink-fitting, hyperelastic materials, and thin-shell buckling. The behavior experienced by many objects and systems in the world can be modeled with a greater degree of accuracy using the nonlinear capabilities of NX Nastran.
Two separate cantilever beams with I-Beam Cross Sections will be used to demonstrate large deformations usually found in Nonlinear Static Analysis. For the beam properties one Standard Cross Section (PBEAM) and one NASTRAN Beam (PBEAML) will be created. The beams will have one end fixed, and the free end will be loaded with a Moment. This example will use the Nonlinear Static solving capability of NX/Nastran.
For this example a beam model will be created using FEMAP. The analysis process includes:
· creating a beam property two separate ways, mesh an existing curves, and viewing the cross-sections of the elements
· creating Moment loads on free ends of I-Beams and fixed constraints
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the large deformations of I-Beams using FEMAP’s Multi-Set Animation capability
Creating the Geometry What Create lines to represent the beams
How
Step 1.
UI Menu
Command/Display File, New
27-2 2.
Large Deformation - Cantilever Beam
Geometry, Curve-Line, Coordinates Menu
3.
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
X = 300, Y = 0, Z = 0, Then…Click OK button
In the Locate – Enter First Location of Line dialog box:
X = 0, Y = 0, Z = 200, Then…Click OK button
In the Locate – Enter Second Location of Line dialog box:
4.
X = 300, Y = 0, Z = 200 Click OK, then
5.
Click Cancel View, Rotate, Model or… Menu
Press the F8 Key 6.
In View Rotate dialog box:
Click Isometric button, then…
Click OK
Note: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
Creating the Materials and Properties
27-3
Creating the Materials and Properties What Create a Material
How
Step 1.
UI
Command/Display Model, Material
Menu
2.
In Define Material - ISOTROPIC dialog box:
Type “I-Beam” in Title field, then…
Enter “200,000” in Young’s Modulus, E field (units: N/mm2)
Enter “0.3” in Poisson’s Ratio, nu field Click OK, then…
3.
Click Cancel
FEMAP has two separate ways to define the cross section of a beam property. Both methods allow the user to pick from a list of “pre-defined cross sections” and enter in specific values for the dimensions. The Standard Beams (PBEAM) also allow the user to create a General Section (choose from any planer surface), choose the stress recovery points, define the orientation of the Y-axis on the property form, and choose to calculate the Shear Center offset and Warping Constant. The NASTRAN Beam (PBEAML) allows changes to the dimension of the beam on the actual PBEAML property input card and always calculates the Shear Center offset and Warping Constant. Both Beams use the Cross Section Y-axis for orientation, but the relationship between the Cross section Y-Axis and Z-Axis are opposite for the two types of beams
What Create the Standard Beam Property
How
Step 1.
UI Menu
Command/Display Model, Property
27-4
Large Deformation - Cantilever Beam
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property button In Element / Property Type dialog box:
4.
Choose Beam radio button in Line Elements section Click OK
5.
In Define Property – BEAM Element Type dialog box:
6.
Type “Standard Beam” in Title field Select “I-Beam” from the Material drop down menu
7.
Click Shape button
8.
In Cross Section Definition dialog box:
9.
Select “I-Beam or Wide Flange (W)” from the Shape drop down menu Enter the following values into the corresponding fields in the Size section of the dialog box:
Height = 8 Width, Top = 8 Width, Bottom = 8 Thick, Top = 0.5 Thick, Bottom = 0.5 Thickness = 0.5 (this is the thickness of the web of the beam)
Click the Draw Section Button to see the defined section Notice: If you choose the “Compute Warping Constant” option when creating a beam cross-section (not used in this example), FEMAP will calculate the warping constant for the cross section. FEMAP bring up this message box when the model using this option is exported for analysis:
Simply click Yes to use the “scalar points” created by FEMAP for post-processing.
Creating the Materials and Properties
10.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel What Create the NASTRAN Cross Section Beam Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – BEAM Element Type dialog box:
Type “NASTRAN Beam” in Title field
27-5
27-6
Large Deformation - Cantilever Beam
3.
Select “I-Beam” from the Material drop down menu
4.
Click Shape button
5.
In Cross Section Definition dialog box:
6.
Choose NASTRAN radio button in upper right corner of dialog box Select “NASTRAN I” from the Shape drop down menu
7.
Enter the following values into the corresponding fields in the Size section of the dialog box:
DIM1 = 8 (Height) DIM2 = 8 (Width, Bottom) DIM3 = 8 (Width, Top) DIM4 = 0.5 (thickness of the web of the I-beam) DIM5 = 0.5 (Thick, Bottom) DIM6 = 0.5 (Thick, Top) Click the Draw Section button to see the defined section Notice: It is very important to hit the Draw Section button, especially with the ambiguity of the dimension (DIM) values when creating the NASTRAN beams to make sure the beam dimensions are accurate.
Creating the Materials and Properties
8.
Click OK, then…
In Define Property – BEAM Element Type dialog box:
Click OK, then…
Click Cancel Meshing the Curves
What Set the mesh size on the curves
How
Step 1.
UI
Command/Display Mesh, Mesh Control, Size Along Curve
Menu
2.
Entity Selection – Select Curve(s) to Set Mesh Size
Choose both curves (curve 1 and 2) 3.
Click OK
4.
In Mesh Size Along Curves dialog box:
5.
Enter “15” in Number of Elements field Click OK, then…
Click Cancel
What Mesh the line
How
Step
UI
Command/Display
27-7
27-8 1.
Large Deformation - Cantilever Beam
Mesh, Geometry, Curve Menu
2.
Entity Selection – Select Curve(s) to Mesh
Choose curve 1
Curve 1
Curve 2
3.
Click OK
4.
In Geometry Mesh Options dialog box:
5.
Select “Standard Beam” from the Property drop down menu Click OK
6.
In the Vector Locate – Define Element Orientation Vector dialog box:
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 0, Z = 1 Click OK
7. 8.
Mesh, Geometry, Curve Menu
9.
Entity Selection – Select Curve(s) to Mesh
Choose curve 2 10.
Click OK
Creating the Materials and Properties
11.
In Geometry Mesh Options dialog box:
12.
Select “NASTRAN Beam” from the Property drop down menu Click OK
13.
In the Vector Locate – Define Element Orientation Vector dialog box:
27-9
Enter: Base X = 0, Y = 0, Z = 0 Tip X = 0, Y = 1, Z = 0
Notice: This is a different orientation vector than was used with the standard beam Property Click OK
14. 15.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 16.
Click Geometry Off button, then…
Click Done Notice: You can use the Entity Display Toolbar to quickly toggle Geometry on and off. If the Entity Display Toolbar is not visible, you can turn it on using the Tools, Toolbars, Entity Display command to make visible (shown “undocked”).
You have the option to toggle ALL Geometry on and off using the first icon or you can turn them on and off individually by clicking the icon for each geometric entity one at a time. Viewing the Beam Cross Sections
What Utilize the View Options to visualize Beam Cross Sections
How
Step 1.
UI
Command/Display View, Options or…
Menu
Press the F6 Key or choose “Options” from the View Style icon
on the View Toolbar
27-10
Large Deformation - Cantilever Beam
2.
In View Options dialog box:
3.
Choose Entities, Labels, and Colors radio button under Category Highlight “Element – Orientation/Shape” from the selection list (This will change the right hand side of the View Options dialog box to have specific options for the highlighted option), then…
Highlight “3..Show Cross Section” from the Element Shape selection list Click OK
4.
Tip: You can also “toggle” the cross-sections of line elements on/off using the “Thickness/Cross Section” command from the View Style menu located on the View Toolbar. The model should now look like this:
Fixed End
Free End
Creating the loads and constraints What Apply fixed constraints to the fixed end of both beams How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating the loads and constraints
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Fixed” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the node at the fixed end of each beam (Nodes 1 and 17) 6.
Click OK
In Create Nodal Constraints/DOF dialog box:
Click Fixed button, then…
Click OK, then…
In Entity Selection – Enter Node(s) to Select dialog box:
Click Cancel What Apply a moment to the free end of each beam
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Moment” in the Title field Click OK
4.
Model, Load, Nodal Menu
27-11
27-12 5.
Large Deformation - Cantilever Beam
Entity Selection – Enter Node(s) to Select dialog box
Select the node at the free end of each beam (Nodes 16 and 32) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Moment from the selection list 8.
Enter “534000” in MZ field (units: Nmm)
9.
Click OK, then…
Click Cancel
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX Nastran through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis.
Running the Nonlinear Static Analysis
27-13
4.
Enter “10” into Number of Increments field
5.
Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step 1.
UI Menu
Command/Display Model, Analysis
27-14
Large Deformation - Cantilever Beam
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Large Deformation” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Large Deformation Results The Nonlinear Static Analysis has been completed. The best way to view the deformation results of the beams is with a deformed plot.
What View the deformation results in a FEMAP deformed plot
How
Step
UI
Command/Display
Post-Processing the Large Deformation Results
1.
27-15
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
3.
Choose Deform radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
from the View Toolbar
Select “Last Analysis Step, Time 1” (Should be Step 21, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in Output Vectors section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting Postprocessing as the Category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Post Options menu on the Post Toolbar for this task
27-16
Large Deformation - Cantilever Beam
The Post Options icon
also has these toggles and options
1. Undeformed: Turn the Undeformed Model On and Off 2. Scale Deformation: Set a Deformation Scale for the Model 3. Animation Frames: Set the number of frames used in Animation 4. Animation – Positive Only: Animate only in the loaded direction 5. Animation – Load and Unload: Animate loading only, then repeat 6. Animate Contours: Animate the contours as the model deforms 7. Filled Contours: Use outlines only for contours 8. Contour Options…: Bring up the Contour Options dialog box 9. Freebody...: Bring up the View Freebody Options dialog box 10. More options…: Bring up the View Options dialog box
Most of these options relate to Animation of one Output Set only. View, Autoscale, Visible
7. Menu
OR Press Ctrl - A The deformed plot of the nodal displacements actual deformation should look like this:
If you would like to toggle the “Undeformed” model on and off to compare the deformed model to the original model, click the Post Options icon on the Post Toolbar and select Undeformed from the drop down list. Animating the Results Using Animate Multi-Set
What View all the Output Sets in one sequential animation
How Step
UI
Command/Display
Post-Processing the Large Deformation Results
1.
27-17
View, Select or… Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate-MultiSet radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Selecting PostProcessing Data dialog box:
Select “1..Case 1 Time 0.05” from Output Set drop down menu
Select “21..Case 21 Time 1” from Final Output Set drop down menu Click OK
5.
In Selecting PostProcessing Data dialog box:
Click OK, then…
In View Select dialog box:
Click OK Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The model should now be animating the deformations one step at a time.
Use the View, Advanced Post, Animation menu command to speed up and slow down the animation.
What Return the model to a deformed plot
How Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
27-18
Large Deformation - Cantilever Beam
2.
In View Select dialog box:
3.
Choose Deformed radio button in Deformed Style section Click OK
This Concludes the Large Deformation example. It is recommended to save the model file.
Slide Line Contact - Hyperelastic Seals 28.
Two semicircular seals are being pressed together at a given enforced displacement. The seals are the same size and shape and the rounded sides of the seals will come into contact with one another. The seals are made of a hyperelastic material and the model allows the use of plane strain elements for analysis. Contact between the rounded sides of each seal will be modeled using Slide Line Contact. Slide line contact differs from Gap contact in that is not simply a point-to-point or nodeto-node representation of contact, but a 2-D relationship between a set of Master nodes and a set of Slave Nodes. This example will use the Nonlinear Static solving capability of NX Nastran.
For this example a model of two seals has already been created. The analysis process includes:
· modifying the hyperelastic material
· creating a Slide Line property and then selecting the Master and Slave sets to create the slide line element for contact
· creating an Enforced Displacement to bring the seals together into contact
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the multi-set animation of the analysis sets to understand how the contact between the seals progresses
Upper Seal
Lower Seal
28-2
Slide Line Contact - Hyperelastic Seals
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Nonlinear/seals.neu Locate seals.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
Modifying the Material
28-3
Modifying the Material The seals need to be made of a hyperelastic material. The model currently has an isotropic material defined. The type of material needs to be selected and the correct Directional and Volumetric Deformation Constants entered for the analysis to run correctly.
What Modify the Material
How
Step 1.
UI
Command/Display Modify, Edit, Material
Menu
2.
In Entity Selection – Select Material(s) to Edit dialog box:
Click OK, then…
In Define Material - ISOTROPIC dialog box:
3.
Click Type button Tip: You can also edit an existing Material using the Edit command on the “context sensitive menu” located on the Materials branch in the Model Info tree (simply click to highlight any existing Material, then right mouse click to see the context sensitive menu). In Material Type dialog box:
4.
Choose Hyperelastic radio button Click OK
5.
In Define Hyperelastic Material dialog box: Type “Hyperelastic” in Title field Enter “100” in Table10 (A10) field in Directional Deformation Constants (Aij) section Enter “0.005” in Table01 (A01) field in Directional Deformation Constants (Aij) section Enter “10000” in first Volumetric Deformation Constants (Di) field
28-4
6.
Slide Line Contact - Hyperelastic Seals
Click OK
Creating the Slide Line Property and Element The Slide Line Element requires a property be defined to include values for Master width, Slave width, Non-Sliding Frictional Stiffness, Static Friction Coefficient and Stiffness Scale Factor. Additionally, the Slide Line Plane can be defined, as well as, a check to specify Unsymmetrical or Symmetrical Penetration.
Here are some additional considerations that should be taken into account when using Slide Line Contact:
· Slide Line Contact must always be used in conjunction with Static or Transient Nonlinear Analysis.
· The XY Plane for Slide Line Contact is always defined by the global or local coordinate system that is referenced in the Slide Line property.
· Master and Slave designation is for naming purposes only in symmetric penetration. When Unsymmetrical Penetration is used, only Slave nodes are checked for penetration into the Master segment
· The Z-axis of the reference coordinate system in the Slide Line Property is used to align the slide line elements. The right hand rule should be taken into account when selecting Master and Slave nodes. Slave and Master segment Normals MUST face each other.
Creating the Slide Line Property and Element
28-5
· When performing Static Nonlinear analysis, try to use an enforced displacement instead of applied loads, if possible, due to better convergence of the model. (Enforced displacement can not be used in Transient Nonlinear Analysis)
What Create the Slide Line Property
How
Step 1.
UI
Command/Display Model, Property
Menu
2.
In Define Property – PLATE Element Type dialog box:
3.
Click Elem/Property Type button In Element / Property Type dialog box:
4.
Choose Slide Line radio button in Other Elements section Click OK
5.
In Define Property – SLIDE LINE Element Type dialog box:
Type “Slide Line” in Title field Enter “1.95” in Master Width field Enter “1.95” in Slave Width field Enter “0.5” in Nonsliding Frictional Stiffness field Enter “0.4” in Static Friction Coefficient field
Notice: The slide line plane used in this analysis in the 0..Basic Rectangular, but a local coordinate system could be generated and referenced for a slide line that does not lie in the Global XY Plane.
Notice: Symmetrical Penetration is often more accurate when contact is occurring between two bodies which allow the same level of penetration, but creates longer computation times than Unsymmetrical Penetration.
28-6
6.
Slide Line Contact - Hyperelastic Seals
Click OK, then…
Click Cancel What Create the Slide Line Element
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
3.
Select “Slide Line” from the Property drop down menu Click Master Nodes button
Creating the Slide Line Property and Element
4.
28-7
Entity Selection – Select Master Nodes
Choose nodes on the lower seal in the following order: (Nodes 183 to 189 and Nodes 254 to 261)
Start Here
5.
End Here
Notice: It is critical to choose the nodes one at a time, in this order for the Slide Line Element to work properly Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click Slave Nodes button
28-8 6.
Slide Line Contact - Hyperelastic Seals
Entity Selection – Select Slave Nodes
Choose nodes on the Upper seal in the following order: (Nodes 100 to 106 and Nodes 6 to 13)
End Here
Start Here
Notice: It is recommended to choose the Slave nodes one at a time, in the reverse order of the Master nodes for the Slide Line Element to work more effectively Click OK
7.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click OK, then…
Click Cancel
Creating the loads and constraints What Apply constraints to the bottom of the Lower Seal to not allow translation in the Y and Z directions, and “fix” the center node in the X-direction as well.
How
Step 1.
UI Menu
Command/Display Model, Constraint, Set
Creating the loads and constraints
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the bottom of the Lower Seal using a box pick:
Node 167 6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY and TZ boxes Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Center node at the bottom of the Lower Seal (Node 167) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
CHECK TX, TY, and TZ boxes
28-9
28-10 12.
Slide Line Contact - Hyperelastic Seals
Click OK, then…
In NX Nastran for FEMAP dialog box:
“Selected Constraints Already Exist. OK to Overwrite (No=Combine)?”
Click Yes, then…
Click Cancel What Apply Enforced Displacements to the top of the Upper Seal
How
Step 1.
UI
Command/Display Model, Load, Set
Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Displacements” in the Title field Click OK
4.
Model, Load, Nodal Menu
Creating the loads and constraints
5.
28-11
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the top of the Upper Seal using a box pick:
6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 8.
Enter “-0.6” in TY field (units: Inches)
9.
Click OK, then…
Click Cancel What Apply constraints to the top of the Upper Seal to not allow translation in the Z direction, and “fix” the center node in the Xdirection as well. Also, in NX Nastran, the degree of freedom in the direction of an Enforced Displacement must be constrained. Therefore, the Y-translation of all the nodes on the top of the Upper seal must be constrained.
How
Step 1.
UI Menu
Command/Display Model, Constraint, Nodal
28-12 2.
Slide Line Contact - Hyperelastic Seals
Entity Selection – Enter Node(s) to Select dialog box:
Select the nodes at the top of the Upper Seal using a box pick:
Node 1
3.
Click OK
4.
In Create Nodal Constraints/DOF dialog box:
5.
CHECK TY and TZ boxes Click OK
6.
Entity Selection – Enter Node(s) to Select dialog box:
Select the Center node at the bottom of the Lower Seal (Node 1) 7.
Click OK
8.
In Create Nodal Constraints/DOF dialog box:
9.
CHECK TX, TY, and TZ boxes Click OK, then…
In NX Nastran for FEMAP dialog box:
“Selected Constraints Already Exist. OK to Overwrite (No=Combine)?”
Click Yes, then…
Click Cancel
Creating Settings for Nonlinear analysis
28-13
The Model should now look like this:
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. First, the type of analysis must be chosen as Static, Creep, or Transient. Many times the Defaults button can be chosen to create the convergence criteria for the model. Also, the number of increments must be entered, iterations allowed per increment, and if an output set is required for all the steps that lead to the final result. Settings such as Solution Strategy Overrides, Stiffness Updates, Creep Criteria, and other Advanced Nonlinear options are also available for NX NASTRAN through FEMAP.
What Create Nonlinear Static settings
How
Step 1.
UI
Command/Display Model, Load, Nonlinear Analysis
Menu
2.
In Load Set Options for Nonlinear Analysis dialog box:
Choose Static radio button
28-14
Slide Line Contact - Hyperelastic Seals
3.
Click Defaults button
4.
Notice: This will fill in some of the fields with “Default Values” for the control parameters of nonlinear static analysis only. If the Defaults button is used it will always assume Nonlinear Static analysis. These “Defaults” are often a great place to begin when performing this type of analysis. Enter “30” into Number of Increments field
5.
Notice: Contact Analysis often requires a higher number of increments to improve convergence of a solution. Select “3..ALL” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
Post-Processing the Slide Line Contact Results
28-15
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Slide Line” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Slide Line Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the seals is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What
28-16
Slide Line Contact - Hyperelastic Seals
View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon In View Select dialog box:
2.
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 37, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “7233..Plate Mid VonMises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Post-Processing the Slide Line Contact Results
28-17
The deformation and stress results should look like this:
Zoom in on the Contact Region:
The Nodes do no meet up exactly as in gap contact because they are allowed to slide along the Slide Line as the model changes shape.
What View the results in a FEMAP Animation of all the analysis sets
28-18
Slide Line Contact - Hyperelastic Seals
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.0333333)” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 37, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model
The Contact between the seals can be viewed in this mode as the seals are pushed together.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This Concludes the Slide Line Contact example. It is recommended to save the model file.
3-D Contact - Plastic Clip and Base 29.
A plastic clip made of solid elements will come into contact with a fixed base and move through a range of motion based on enforced displacements using slide line contact.
For this example the clip and the base have already been created. The analysis process includes:
· creating Slide Line elements by selecting the Master and Slave node sets for contact
· creating an Enforced Displacement to bring the Clip into contact with the Base
· defining the analysis parameters to aid in convergence of the Nonlinear solution
· analyzing the model with NX Nastran’s Nonlinear Static Solution Method
· viewing the multi-set animation of the analysis sets to understand the contact between the objects.
Plastic Clip
Fixed Base
29-2
3-D Contact - Plastic Clip and Base
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, and Materials
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Nonlinear/snapfit.neu Locate snapfit.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are solid 3-D elements.
Creating the Contact (Slide Line) Element
29-3
Creating the Contact (Slide Line) Element What Create the Slide Line Element
How
Step 1.
UI
Command/Display Model, Element
Menu
2.
In Define PLATE Elements – Enter Nodes or Select with Cursor dialog box:
3.
Click Type button In Element / Property Type dialog box:
4.
Choose Slide Line radio button in Other Elements section Click OK
5.
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
6.
Select “Slide Line” from the Property drop down menu Click Master Nodes button
7.
In Entity Selection – Select Master Nodes dialog box:
Click Pick button, then select Front from the menu
Notice: This will allow the user to choose the entity that is in front of other entities. The screen is always the XY plane in this command, so the entity that is in the “front” is the entity that has the highest value in the “Z-direction” (perpendicular to the XY plane of the screen).
29-4 8.
3-D Contact - Plastic Clip and Base
Choose nodes on the fixed base in the following order: (Nodes 1145 to 1179)
End Here
Start Here
9.
Notice: It is critical to choose the nodes one at a time, in this order for the Slide Line Element to work properly. Also, be sure that only one node is chosen at each location, the slide line property specifies the XY Plane used and any nodes chosen outside that plane will cause the analysis to end without running. Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
10.
Click Slave Nodes button Entity Selection – Select Slave Nodes Choose nodes on the Plastic Clip in the following order: (Nodes 30 to 31, 557-571, 422-435, and Node 53)
Start Here
End Here
Notice: It is recommended to choose the Slave nodes one at a time, in the reverse order of the Master nodes for the Slide Line Element to work more effectively
Creating the Contact (Slide Line) Element
11.
29-5
Click OK
In Define SLIDE LINE Element – Enter Nodes or Select with Cursor dialog box:
Click OK, then…
In NX Nastran for FEMAP dialog box:
Click NO (The elements were selected in the correct order, so the selection order does not need to be reversed), then...
Click Cancel The Model should now look like this:
Creating the permanent constraints
For this example every node will have some degrees of freedom permanently constrained in order for the analysis to run correctly and more efficiently. For example the base will be fixed for the duration of the analysis and is assumed to be undeformable. Therefore, all the nodes of the base will be permanently constrained. Because of this, stress values will only be calculated for the plastic clip.
What Create Permanent Constraints on multiple nodes with one command.
How
29-6
Step 1.
UI
3-D Contact - Plastic Clip and Base
Command/Display Modify, Update Other, Perm Constraint
Menu
2.
In Entity Selection – Select Node(s) to Update Permanent Constraints dialog box:
Click Select All, then…
3.
Click OK In Update Nodal Permanent Constraints dialog box:
CHECK TZ, RX, and RY boxes
4.
Click OK
5.
In Entity Selection – Select Node(s) to Update Permanent Constraints dialog box:
Choose all the nodes of the fixed base with a box pick (Hold Shift and drag a box around the fixed base)
Creating the loads and constraints
6.
29-7
In Update Nodal Permanent Constraints dialog box:
CHECK TX, TY, TZ, RX, RY and RZ boxes
7.
Click OK
Creating the loads and constraints What Apply constraints to the bottom of the Clip to not allow translation in the Y direction, and “fix” the loaded nodes in the X Translation direction as well. In order for NX Nastran to use enforced displacements, the degree of freedom in the direction of the enforced displacement must be constrained.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Model, Constraint, Nodal Menu
29-8 5.
3-D Contact - Plastic Clip and Base
Entity Selection – Enter Node(s) to Select dialog box:
Select the 6 nodes shown at the bottom of the Clip using a box pick: (Nodes 74-76 and 730-732)
Nodes to be constrained in TY
6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY box Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Nodes to be constrained in TX and TY
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
12.
CHECK TX and TY boxes Click OK, then…
Click Cancel What Apply Enforced Displacements to the nodes constrained in both X and Y Translation in the step above (nodes 73 and 729)
How
Step
UI
Command/Display
Creating Settings for Nonlinear analysis
1.
29-9
Model, Load, Set Menu
2.
In Create or Activate Load Set dialog box:
3.
Type “Displacements” in the Title field Click OK
4.
Model, Load, Nodal Menu
5.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 6.
Click OK
7.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 8.
Enter “2.25” in TX field (units: Inches)
9.
Click OK, then…
Click Cancel
Creating Settings for Nonlinear analysis Certain settings need to be defined in order for a nonlinear analysis to run. For this Nonlinear Static analysis the number of increments will be set to a larger number than many of the previous examples in order to aid solution convergence.
What Create Nonlinear Static settings
How
Step 1.
UI Menu
Command/Display Model, Load, Nonlinear Analysis
29-10
3-D Contact - Plastic Clip and Base
2.
In Load Set Options for Nonlinear Analysis dialog box:
3.
Choose Static radio button Click Defaults button
4.
Enter “75” into Number of Increments field
5.
Notice: Contact Analysis often requires a higher number of increments to improve convergence of a solution. Select “1..Yes” from the Intermediate drop down menu in the Output Control section
6.
Click OK
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Nonlinear Static Analysis using the FEMAP Analysis Set Manager
Post-Processing the Slide Line Contact Results
29-11
How Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Enter “Snapfit” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “10..Nonlinear Static” from the Analysis Type drop down menu
5.
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Slide Line Contact Results The Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multiset Animation.
What View the results in a FEMAP contour plot of a deformed model
29-12
3-D Contact - Plastic Clip and Base
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon In View Select dialog box:
2.
from the View Toolbar
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 83, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “60031..Solid Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon the drop down list
from the Post Toolbar and select Actual Deformation from
Post-Processing the Slide Line Contact Results
29-13
The deformation and stress results should look like this:
What View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.0333333)” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 83, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically.
29-14 5.
3-D Contact - Plastic Clip and Base
Click OK, then…
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The Contact between the Clip and the Base can be viewed in this mode as the objects come into contact.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the 3-D Contact example. It is recommended to save the model file.
Large Deformation - Advanced Nonlinear (SOL 601) 30.
A small part made of plate elements will be subjected to a functionally-dependent load and experience large deformation.
For this example the part already been created. The analysis process includes:
· creating a functionally-dependent Load to create large deformation.
· defining the analysis parameters for the Nonlinear solution (Analysis Set Manager)
· analyzing the model with NX Nastran’s Advanced Nonlinear Solution (SOL 601)
· viewing the deformed plot and multi-set animation of the analysis sets to see the large deformation.
Part
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, Materials, and Constraints
30-2
Large Deformation - Advanced Nonlinear (SOL 601)
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Advanced_Nonlinear/Large601.neu Locate Large601.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are Plate Elements. The nodes at the bottom edge of the part are fixed in all degrees of freedom.
Creating the functionally dependent loads
30-3
Creating the functionally dependent loads What Apply functionally dependent Forces to nodes opposite the constrained edge in the positive Z direction. The function will be used to “step” the load up as the analysis progresses.
How
Step 1.
UI
Command/Display Model, Function
Menu
2.
In Function Definition dialog box:
3.
Type “Loading Function” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Linear Ramp radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 1 Delta X = 0.05 Y = 0.0 To Y = 1
30-4 6.
Large Deformation - Advanced Nonlinear (SOL 601)
Click More button
X and Y Values will be created for the function.
7.
Note: This will produce values from 0 to 0.95. A final data point will be added to insure the load has been fully applied. Choose Single Value radio button
8.
Enter the following values in the corresponding fields:
9.
X =1.0 Y = 1.0 Click OK, then…
10.
Click Cancel Model, Load, Set Menu
11.
In Create or Activate Load Set dialog box:
12.
Type “Forces” in the Title field Click OK
13.
Model, Load, Nodal Menu
14.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 3 nodes on the edge opposite the constrained edge (Nodes 55, 56, and 57).
Running the Nonlinear Static Analysis
15.
Click OK
16.
In Create Loads on Nodes dialog box
Highlight Force from the selection list 17.
Enter “1333.3” in FZ field
18.
Select “1..Loading Function” from Time/Freq Dependence drop down menu.
19.
Click OK, then…
Click Cancel The Model should now look like this:
THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Advanced Nonlinear Static Analysis using the FEMAP Analysis Set Manager
How
Step
UI
Command/Display
30-5
30-6 1.
Large Deformation - Advanced Nonlinear (SOL 601)
Model, Analysis Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Large 601” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “22..Advanced Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next button 2 times
6.
In NASTRAN Bulk Data Options dialog box:
CHECK LGDISP box
7.
Note: This PARAM in NX Nastran is very important for Large Displacement Analysis. Without the PARAM answers will be considerably different and inaccurate. Click Next button 3 times
8.
In NXSTRAT Solver Parameters dialog box
Enter “20” in the Number of Steps field in the Time Steps section
Enter “0.05” in the Time Increment field in the Time Steps section
Running the Nonlinear Static Analysis
9.
Click Next button 1 time
10.
In NXSTRAT Iteration and Convergence Parameters dialog box
30-7
Select “1..On” from the Auto Increment drop down menu in the Analysis Control section.
30-8
11.
Large Deformation - Advanced Nonlinear (SOL 601)
Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Large Deformation Results The Advanced Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
Press the F5 Key or choose the view select icon
from the View Toolbar
Post-Processing the Large Deformation Results
2.
30-9
In View Select dialog box:
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
4.
In Select PostProcessing Data dialog box:
Select “20..Case 20 Time 1.” (Should be Step 20, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “7033..Plate Top Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the Post Toolbar and select Actual Deformation from the drop down list (Must have a check mark next to it in the menu)
7.
Ctrl+A
Ctrl+A will perform the View, Autoscale, Visible command.
Note: Use the magnify down icon on the View Toolbar or spin the wheel of a wheel mouse until the entire deformed image can be seen.
30-10
Large Deformation - Advanced Nonlinear (SOL 601)
The deformation and stress results should look like this:
What
View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
Post-Processing the Large Deformation Results
4.
30-11
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.01)” from drop down menu located in the Output Set section
Select “20..Case 20 Time 1.” (Should be 20, but may differ based on machine set-up) from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The part can now be viewed as it experiences large deformation.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the Large Deformation - Advanced Nonlinear (SOL 601) example. It is recommended to save the model file.
30-12
Large Deformation - Advanced Nonlinear (SOL 601)
Surface to Surface Contact Advanced Nonlinear (SOL 601) 31.
A clip made of solid elements will come into contact with a fixed base and move through a range of motion based on enforced displacements using surface to surface contact.
For this example the clip and the base have already been created. Also, permanent constraints and the contact segments have also been created to focus the example on performing the analysis. The analysis process includes:
· creating the Connection Property and defining the Connector for surface to surface contact in NX Nastran.
· creating a functionally-dependent Enforced Displacement to bring the Clip into contact with the Base
· defining the analysis parameters to aid in convergence of the Nonlinear solution (Analysis Set manger)
· analyzing the model with NX Nastran’s Advanced Nonlinear Solution (SOL 601)
· viewing the multi-set animation of the analysis sets to understand the contact between the objects.
Plastic Clip
Base
31-2
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
Importing the Neutral File What Import a FEMAP neutral file containing the Nodes, Elements, Properties, Materials, Permanent Constraints, and Connection Regions
How
Step 1.
UI
Command/Display File, New
Menu
2.
File, Import, FEMAP Neutral Menu
3.
Read Model from FEMAP Neutral dialog box:
4.
FEMAP93/Examples/Advanced_Nonlinear/snap601.neu Locate snap601.neu
Click Open
In Neutral File Read Options dialog box:
Click OK
These Elements are solid 3-D elements.
Creating the Contact Conditions
31-3
Creating the Contact Conditions In order for surface to surface contact to occur during analysis with NX Nastran Advanced Nonlinear Method (SOL 601), several parameters must be defined. In general, Connection Regions are created, a Connection Property is defined, and then a Connector (“contact pair”) is created to define the contact relationship between the two Connection Regions. First, Connection Regions must be created using the Connect, Connection Region command. While this dialog box is open, elements and element faces can be chosen to represent the areas on different parts in the model that will come into contact with one another. The process consists of choosing all elements around the outside edge of a part that may possibly come into contact with another part. Once these elements are chosen, an element face must be chosen to allow NX Nastran to know what face of the element will be part of a contact surface. When all the elements have be chosen and faces selected, the Connection Region will, by default, be shown as orange colored “plate elements” with thick orange edges on the screen. For this model, the Connection Regions have been created to save modeling time and focus on the use of the NX Nastran Advanced Nonlinear solution sequence (SOL 601). Viewing the Connection Regions will show how these regions should be created. The regions in this model were created by choosing the Elements radio button then clicking the Multiple button in the Define Connection Region dialog box. Multiple allows a number of elements around the edge of the part to be chosen at the same time, then element faces are selected using the Adjacent Faces option in the Face Selection for Elemental Loads dialog box. What Viewing the Connection Regions
How
Step 1.
UI Crtl-Q
Command/Display This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 2.
In View Quick Options dialog box:
3.
Click All Entities Off button CHECK Connection Region box located in the Others section, then...
4.
Click Done
This will make only the contact segments visible on the screen. These segments will be used along with a contact property to create a contact pair to be used for surface to surface contact. Rotate the View to be able to see the element faces which make up the contact segments.
Deformable
Rigid
31-4
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
After the Connection Regions have been created and visually confirmed, the next step in creating a Connector (contact pair) is creating the Connection Property. Because this type of property is unique, it will only be found as command on the Connect menu. There are three type of contact used by SOL 601 which FEMAP supports: Constraint Function, Segment Method, or Rigid Target. Along with each type of contact there a number of parameters which can be set to define the behavior of the parts that will come into contact. The contact type is usually determined by the type of problem trying to be solved. Also, birth time and death time for a Connection Regions can be defined. For more information on the options see Section 4.4 Creating Connections (NX Nastran Contact Properties) of the FEMAP Commands manual or the Theory and Modeling guide of SOL 601. In this case, the Constraint Function type of contact will be used with the default values assigned.
What Create the Connection Property
How
Step 1.
UI
Command/Display Connect, Connection Property
Menu
2.
Tip: You can also create a new Connection Property using the New command on the “context sensitive menu” located on the Connection Property branch in the Model Info tree (simply click to highlight the top level of the Connection Properties branch or any existing Connection Property, then right mouse click to see the context sensitive menu). In Define Connection Property dialog box:
Type “Contact” in the Title field 3.
Click the NX Adv Nonlin tab in the Define Connection Property dialog box
4.
Make sure that “0..Constraint Function” is selected from the Contact Type drop down menu in the General section.
5.
Also, make sure that Connect Type is set to “0..Contact” (This drop-down is located in the upper right corner of the Define Connection Property dialog box) Click OK, then...
Click Cancel Finally, once the Connection Property has been defined, the Connector (contact pair) can be created. In order to create a Connector, a “Master” Connection Region and a “Slave” Connection Region must be chosen from available Connection Regions. In this model, the Connector will be created to minimize convergence time during the solution. What Create the Connector (contact pair)
Creating the Contact Conditions
31-5
How
Step 1.
UI
Command/Display Connect, Connector...
Menu
2.
In the Define Contact Connector - Select Connection Regions dialog box:
Choose “1..Contact” from the Property drop-down list.
Choose “1..Deformable” from the Master drop-down list.
Choose “2..Rigid” from the Slave drop-down list. Click OK
3. 4.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar 5.
CHECK Element box located in the Others section, then
6.
Click Load/Constraint On
Click Done
7.
Crtl-R
This will show the elements and contact segments only. A single line element will be shown from contact segment to contact segment to represent a contact pair exists between the segments. This will bring up View Rotate dialog box:
OR F8 key 8.
Click XY Top, then...
Click OK Tip: You can also use the View Orient Toolbar to have one click access to several frequently used views. You can turn on this toolbar using Tools, Toolbars, View Orient
31-6
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
The Model should now look like this:
Creating the loads and constraints What Apply constraints to the bottom of the Clip to not allow translation in the Y direction, and “fix” the nodes which will be loaded with the functionally-dependent Enforced Displacement in the X-direction as well.
How
Step 1.
UI
Command/Display Model, Constraint, Set
Menu
2.
In Create or Activate Constraint Set dialog box:
3.
Type “Constraints” in the Title field Click OK
4.
Tip: You can also create a new Constraint Set using the New command on the “context sensitive menu” located on the Constraints branch in the Model Info tree (simply click to highlight the top level of the Constraints branch or any existing Constraint Set, then right mouse click to see the context sensitive menu). Model, Constraint, Nodal Menu
Creating the loads and constraints
5.
31-7
Entity Selection – Enter Node(s) to Select dialog box:
Select the 6 nodes shown at the bottom of the Clip using a box pick: (Nodes 74-76 and 730-732)
Nodes to be constrained in TY
6.
Click OK
7.
In Create Nodal Constraints/DOF dialog box:
8.
CHECK TY box Click OK
9.
Entity Selection – Enter Node(s) to Select dialog box:
Nodes to be constrained in TX and TY
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 10.
Click OK
11.
In Create Nodal Constraints/DOF dialog box:
12.
CHECK TX and TY boxes Click OK, then…
Click Cancel What Apply functionally dependant Enforced Displacements to the nodes constrained in both the X and Y Translation directions in the last step. The function will be used to “step” the displacement load up as the analysis progresses.
How
Step
UI
Command/Display
31-8 1.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
Model, Function Menu
2.
In Function Definition dialog box:
3.
Type “Loading function” in Title field Select “1..vs. Time” from Type drop down menu.
4.
Choose Linear Ramp radio button
5.
Enter the following values in the corresponding fields:
X = 0.0 To X = 1 Delta X = 0.01 Y = 0.0 To Y = 1 6.
Click More button
X and Y Values will be created for the function.
7.
Note: This will produce values from 0 to 0.99. A final data point will be added to insure the load has been fully applied. Choose Single Value radio button
Running the Nonlinear Static Analysis
8.
Enter the following values in the corresponding fields:
9.
X =1.0 Y = 1.0 Click OK, then…
10.
Click Cancel Model, Load, Set Menu
11.
In Create or Activate Load Set dialog box:
12.
Type “Displacements” in the Title field Click OK
13.
Model, Load, Nodal Menu
14.
Entity Selection – Enter Node(s) to Select dialog box:
Select the 2 nodes on the right side of the bottom of the Clip: (Nodes 73 and 729) 15.
Click OK
16.
In Create Loads on Nodes dialog box
Highlight Displacement from the selection list 17.
Enter “2.25” in TX field (units: Inches)
18.
Select “1..Loading Function” from Time/Freq Dependence drop down menu.
19.
Click OK, then…
Click Cancel THE MODEL IS NOW READY TO BE ANALYZED!
Running the Nonlinear Static Analysis What Create an analysis case for Advanced Nonlinear Static Analysis using the FEMAP Analysis Set Manager
31-9
31-10
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
How
Step 1.
UI
Command/Display Model, Analysis
Menu
2.
In Analysis Set Manager dialog box:
3.
Click New button In Analysis Set dialog box
4.
Type “Snapfit 601” in the Title field Select “36..NX Nastran” from the Analysis Program drop down menu, then…
Select “22..Advanced Nonlinear Static” from the Analysis Type drop down menu
5.
Click Next button 2 times
6.
In NASTRAN Bulk Data Options dialog box:
7.
CHECK LGDISP box Click Next button 3 times
8.
In NXSTRAT Solver Parameters dialog box
Enter “100” in the Number of Steps field in the Time Steps section
9.
Enter “0.01” in the Time Increment field in the Time Steps section Click Next button 1 time
Post-Processing the Surface to Surface Contact Results
31-11
10.
In NXSTRAT Iteration and Convergence Parameters dialog box
11.
Select “1..On” from the Auto Increment drop down menu in the Analysis Control section. Click OK, then…
In Analysis Set Manager dialog box:
Click Analyze
Upon Completion of the Analysis, FEMAP will ask “OK to read Nonlinear Stresses and Strains?”...Click Yes
Post-Processing the Surface to Surface Contact Results The Advanced Nonlinear Static Analysis has been completed. The best way to view the deformation and stress results of the plastic part is a contour plot. After the contour Plot of the final step is viewed, watch the contact progress with a contoured Multi-set Animation.
What View the results in a FEMAP contour plot of a deformed model
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
Choose Deform radio button in Deformed Style section
3.
Choose Contour radio button in Contour Style section Click Deformed and Contour Data button
from the View Toolbar
31-12 4.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
In Select PostProcessing Data dialog box:
Select “Last Analysis Step, Time 1” (Should be Step 75, but may differ based on machine set-up) from drop down menu located in the Output Set section
Select “1..Total Translation” from Deformation drop down menu located in the Output Vector section
Select “60031..Solid Von Mises Stress” from Contour drop down menu located in the Output Vector section Click OK, then…
5.
In View Select dialog box:
Click OK Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below)
6. Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the Post Toolbar and select Actual Deformation from the drop down list (Must have a check mark next to it in the menu)
If the “Undeformed model” is already NOT visible, skip this portion of the step:
Click the Post Options icon from the Post Toolbar again and select Undeformed from the drop down list (Must NOT have a check mark next to it in the menu)
Post-Processing the Surface to Surface Contact Results
The deformation and stress results should look like this:
What
View the results in a FEMAP Animation of all the analysis sets
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Animate – Multi-Set radio button in Deformed Style section Click Deformed and Contour Data button
31-13
31-14 4.
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
In Select PostProcessing Data dialog box:
Select “1..Case 1 Time 0.01” from drop down menu located in the Output Set section
Select “Last Analysis Step (Should be 75, but may differ based on machine set-up)” from drop down menu located in the Final Output Set section or leave it Blank and FEMAP will use the Final Analysis Set in the model automatically. Click OK, then…
5.
In View Select dialog box:
Click OK, then Press Ctrl-A to Autoscale the Model Tip: You can use the Model Info tree to quickly create a multi-set animation. Simply expand the Results branch so all the Output Sets in the model are visible in a list. Highlight the Output Set you want to use as the first step in the multi-set animation in the list, then hold down the Shift Key and highlight the Output Set you want to use as the final step in the multi-step animation. Now click the right mouse button on one of the highlighted Output Sets and choose MultiSet Animate from the “context sensitive menu” for Results. The Contact between the Clip and the Base can be viewed in this mode as the objects come into contact.
How
Step 1.
UI
Command/Display View, Select or…
Menu
2.
Press the F5 Key or choose the view select icon In View Select dialog box:
from the View Toolbar
3.
Choose Deform or None-Model Only radio button in Deformed Style section to stop the animation Click OK
This concludes the Surface to Surface Contact - Advanced Nonlinear (SOL 601) example. It is recommended to save the model file.
32.
Analysis of a Simple Assembly
In this example, you will create a model of a simple assembly using contact conditions automatically generated by FEMAP, then solve the model two times using NX Nastran, once using “Glued Contact” and once using “Linear Contact”. Also, this example makes extensive use of the Model Info tree and Select Toolbar.
You will work through the entire FEMAP analysis process, which includes: •
importing the geometry of the assembly
•
creating connections between different parts of the assembly
•
meshing the model
•
applying constraints and loads
•
analyzing the model using the NX Nastran solver (Glued and Linear)
•
post-processing the results
Importing the Geometry What Import a FEMAP geometry file containing the geometry of the assembly.
How Step
UI
Command/Display
1.
File, Import, Geometry Menu
Go to the FEMAP Examples directory. Import the Assembly.x_t file.
32-2 Step
UI
Analysis of a Simple Assembly
Command/Display
2.
Solid Model Read Options dialog box: OK
3.
View, Rotate, Model Menu
Tip: You can press the F8 key instead of using the command above. 4.
View Rotate dialog box: Trimetric OK
Creating Connections You will be creating connections between the different parts of the assembly. In this example, the connections will be contact conditions which NX Nastran will use during the solving process to have the parts interact with one another. In general, there are three separate entities needed to create a connection in FEMAP: Connection Property - A specific property used to set-up contact conditions for a specific solver or analysis type. We will be using the “NX Linear” tab and the Defaults button for this example. Connection Regions - Regions designated in the model which can be placed into contact with any number of other regions. Regions can be created using different types of entities such as surfaces, elements, and properties. In this example, you will create contact between the different solid parts using the surfaces of those solids. Connectors - Connectors create “contact pairs” between Connection Regions (using a Master/Slave relationship) and the contact between those regions is governed by the values set in the specified Connection Property for each Connector. Each of these entities can be created individually using the Connect menu, but FEMAP offers a few methods for creating them in a more streamlined manner. One method is to use the Connect, Surfaces command which simply allows you to choose a surface (or set of surfaces) to “connect” to another surface (or set of surfaces). The surfaces in each set will be used to create the Connection Regions, a Connection Property can be chosen (or created from inside this command), and then a single Connector will be created between the selected surfaces.
Automatic Connection Creation
32-3
In this example, we will be using the Connect, Automatic command. This creates connections automatically based on the proximity of geometric entities selected in your model using a number of parameters. These parameters include specific values for Tolerance (distance between bodies) and Angle Tolerance, as well as choice of a “Detection Strategy” (Minimal to Aggressive) and options for the way multiple Connection Regions will be combined on the same solid.
Automatic Connection Creation What Create connections automatically between the parts of the assembly.
How Step
UI
Command/Display
1.
Connect, Automatic... Menu
2.
Entity Selection dialog box: Select All OK The Auto Detection Options for Connections dialog box, should have the following values selected:
If it does not, make sure all of the above options are chosen. Then... 3.
Click OK In the Entity Selection dialog box: Click Cancel
32-4 Step
UI
Analysis of a Simple Assembly
Command/Display Tip: Creating connections automatically can also be accomplished by using the “context sensitive menu” for the Geometry branch in the Model Info tree. Simply highlight the top-level Geometry branch in the tree (or individual solids), then click the right mouse button and choose Automatic Connection from the menu. This will bring up the Connect, Automatic command
You will notice the there are new Connection Regions which are visible where the parts come together.
You can take a closer look at each Connection Property, Connection Region, and Connector which were created using the Connections branch of the Model Info tree.
Examining Created Connections Using a few “context sensitive menu” commands from the Connections branch of the Model Info tree, you can graphically see the different Connection Regions and Connectors which were created by the Connect, Automatic command. If it is not open, you will need to have the Model Info tree open for this step.
What Use the Model Info tree to examine the connections in the model.
Examining Created Connections
32-5
How Step
UI
Command/Display
1. Menu
If the Model Info tree is NOT already open, you can bring it up using the Tools, Model Info command to make it visible.
Tip: If you are not familiar with the Model Info tree or the other “dockable panes” in FEMAP, you can find more information about them using the Help, Dockable Panes... menu. The “dockable panes” contain a tremendous amount of features. It is highly recommended to take a look at the documentation for these very helpful tools. 2.
In the Model Info tree, expand the Connections branch (click on the “+” sign to the right of the title) to see the different Connection entities
You will notice that Connection Properties, Connection Regions, and Connectors are all available in the Model Info tree. 3.
Expand the Connectors branch to view the Connectors in the model
You will notice that two Connectors were created in the model by the automatic contact detection. They are listed in the following format: #(number of Connector)..Region “#-#” (“Master” Connection Region - “Slave” Connection Region). Highlight “1..Region 1-2” by clicking on it.
32-6 Step 4
UI
Analysis of a Simple Assembly
Command/Display Click the right mouse button on the highlighted Connector. When the “context sensitive” menu appears, choose the Show Master command.
You will notice that the “Master” Connection Region of Connector “1” has been highlighted in Yellow and labeled and the rest of the parts have been made transparent in the model. If your display does not look like the one below, please see the “notice” below this cell.
The model will remain in this display state until Windows, Regenerate (Ctrl+G) has been used or a command which includes a “Regenerate” (such as an entity creation command) has been performed. Notice: The Show Master and Show Slave commands follow the current settings in the Windows, Show Entities command. By default, nothing is set in FEMAP and you will get the figure above when using the Show Master and Show Slave commands. If you have changed any of the settings in the Windows, Show Entities command itself or the Show When Selected commands in the Model Info tree or Data Table, then the Show Master and Show Slave commands will use those settings.
Examining Created Connections
Step 5
UI
32-7
Command/Display Click the right mouse button on the highlighted Connector. When the “context sensitive” menu appears, choose the Show Slave command.
Tip: Although it does not matter for this model, in some cases you may want to “swap” the “Master” and “Slave” Connection Regions. This can be accomplished by using the Reverse command in the Connectors “context sensitive” menu
Tip: It is also possible to “Enable” and “Disable” Connectors in FEMAP. This allows you to choose which Connectors will be exported out of FEMAP for analysis. With this capability, you do not have to delete and recreate Connectors when determining which parts should be coming into contact in certain scenarios.
32-8
Analysis of a Simple Assembly
Applying Loads and Constraints For loads, create a load on front surface of the “Plunger”, normal to the surface. Next, create a “pinned” boundary condition using the surfaces of the rear holes of the “Baselink”.
What Create a load set, then apply a force “normal” to the front surface of the “Plunger”.
How Step
UI
Command/Display
1.
Model, Load, Set Menu
2.
Create or Activate Load Set dialog box: Title: Normal Force
3.
Click OK
For the selection of the surface to load, use the Select Toolbar (Shown Undocked)
If the Select Toolbar is not visible, you can make it visible using the Tools, Toolbars, Select command or by right-mouse clicking in any area where a toolbar can be “docked” and choosing Select from menu. For more information on where a toolbar can be “docked”, please use the Help, Toolbars, Using the Toolbars command to view the documentation. All of the icons on the Select Toolbar are actually menus which allow you to modify the way the Select Toolbar will be used. For more information on the Select Toolbar, please view the documentation specifically created for it using the Help, Toolbars, Select command. 4. Menu
Using the Selector Entity menu on the Select Toolbar (first icon), select Surface. You will notice that the icon on the Select Toolbar has changed to the Select Surface icon.
This will make Surfaces “Active” in the Selector. Having an “Active” entity in the Selector allows you to choose Surfaces in the model before selecting any commands. In this case you will only be selecting one surface at a time, but there are options for selecting multiple surfaces, then choosing commands. This also will give you access to the “context sensitive menu” for the “Active” Entity Type in the graphics window.
Applying Loads and Constraints
Step 5.
UI
32-9
Command/Display With Surface “Active” in the Select Toolbar: Pick the front round surface of the “Plunger” (surface 36). If you turn on the Entity Info dockable pane, you will be able to see which surfaces you are choosing as you pick them. Use the Tools, Entity Info command to open up this pane.
Note: The surface will NOT change color (This has been done for this example to show which surface to select), but the small “Selected Marker” (circle in above figure) will appear in FEMAP to let you know the surface has been selected. 6.
Click the right mouse button on the highlighted Surface or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Load command. This will bring up the Create Loads on Surfaces dialog box. Tip: When the Select Toolbar has an “Active” entity type, a right mouse click in the graphics window will always bring up the “context sensitive menu” for the “Active” Entity Type. Because of this, you will not be able to use the “normal right-mouse menu” simply by clicking the right-mouse button. Instead you have to hold down the Alt key, then click the rightmouse button to get to the “normal right-mouse menu”. When there is no longer an “Active” Entity Type in the Select Toolbar, holding down Alt is not required. Tip: You can also use icons from various toolbars to perform commands on the entities in the currently in the Selector. In this case, you could have used the Create Load on Surface icon on the Loads Toolbar. Create Load on Surface icon
7.
In the Create Loads on Surfaces dialog box: Choose Force from the list of loads, if it is not already chosen.
8.
In the Direction section of the Create Loads on Surfaces dialog box: Select Normal to Surface
32-10 Step
UI
Analysis of a Simple Assembly
Command/Display
9.
In the Load section of the Create Loads on Surfaces dialog box, enter the following value: Magnitude: 100
10.
Click OK
What Create a constraint set, then create “pinned” constraints on the surfaces of the rear holes of the “Baselink”.
How Step
UI
Command/Display
1.
Model, Constraint, Set Menu
2.
Title: Pinned
3.
Click OK
4. Menu
Surfaces should still be the “Active” entity type in the Select Toolbar. If there is no “Active” entity, use the Selector Entity menu on the Select Toolbar (first icon) to select Surface.
Tip: The Select Toolbar remembers the last entity type which was “Active” and a shortcut to make that entity “Active” again is to simply click the Selector Entity icon. Once you are done using the Select Toolbar, click the icon again and it will toggle back to the “no active entity” icon. This is very helpful when going back and forth between using the select toolbar and using FEMAP in the more “traditional” manner (i.e. selecting commands, then entities, then performing the actual command).
Applying Loads and Constraints
Step
UI
32-11
Command/Display
5.
Using the Selector Mode menu (second icon on the Select Toolbar), choose Select Multiple. Menu
This will allow you to choose multiple entities of the current “Active” entity types and create a “Selection List”. You can actually change the “Active” entity and place multiple entities of different types into the same Selection List. Tip: The Selection List can be viewed at the bottom of the Model Info tree. The entity types currently in the Selection List will be listed and the number of each entity type currently in the list will be shown in parenthesis after the entity type name
If you right-click any entity type in the Selection List, you will notice the same “context sensitive menu” will appear for each entity type, as when the entity type is active in the Select Toolbar. This can be an excellent way to get to commonly used commands when you are performing operations on different entity types.
32-12 Step 6.
UI
Analysis of a Simple Assembly
Command/Display With Surface “Active” in the Select Toolbar: Pick the 4 surfaces of the rear holes of the “Baselink” (surfaces 1, 2, 31, and 32).
Note: The surfaces will NOT change color (This has been done for this example to show which surfaces to select), but the small “Selected Markers” (circles in above figure) will appear in FEMAP to let you know the surfaces have been selected. 7.
Click the right mouse button on any of the highlighted Surfaces or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Constraint command. This will bring up the Create Constraints on Surfaces dialog box.
8.
Create Constraints on Geometry dialog box: Pinned - No Translation
9.
Click OK
Meshing the Model
32-13
Meshing the Model You will be using the Model Info tree to select the solids to mesh and then a command from the Solid “context sensitive menu” to actually mesh the assembly. This will reduce the number of commands needed to create the mesh by prompting you to create a material and automatically creating the correct type of property required for solid tetrahedral meshing.
What Mesh the solids using the Model Info tree.
How Step 1.
UI
Command/Display In the Model Info tree, expand the Geometry branch (click on the “+” sign to the right of the title) to see the different Geometry entities (only Solids are in the tree)
Highlight all of solids by selecting the first solid in the list (1..Baselink), then holding the Shift key down and selecting the last solid in the list (3..Pin). 2.
Click the right mouse button on the highlighted Solids. When the “context sensitive menu” appears, choose the Tet mesh command.
32-14 Step
UI
Analysis of a Simple Assembly
Command/Display
3.
FEMAP will prompt you to make a material to be used for all of the selected Solids Define Material - ISOTROPIC dialog box: Click Load
4.
Select from Library dialog box: AISI 4340 Steel (select)
5.
Click OK, then... In the Define Material - ISOTROPIC dialog box: Click OK Tip: You will notice that the model has been sized for meshing. If you want to change the mesh size to anything but the default value, you can do this by clicking the Update Mesh Sizing button in the Automesh Solids dialog box. For this example, the default mesh size is fine.
6.
In the Automesh Solids dialog box: OK The model is now meshed and now is a good time to turn off the Geometry and some other entities in the graphics window.
7.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
8.
In View Quick Options dialog box: Click All Entities Off button, then...
9.
CHECK Element box located in the Mesh section, then
10.
Click Done
Notice: The Loads and Constraints are still applied to the model, they are just no longer visible. If you want to turn then on to verify they are there, simply use Ctrl+Q again and press the Load/Constraint On button and then Done. For this example, we are turning them off now for Post-Processing after the model has been solved.
Analyzing the “Glued Contact” Model
Step
UI
32-15
Command/Display
THE MODEL IS NOW READY TO BE ANALYZED!
Analyzing the “Glued Contact” Model The FEMAP analysis manager stores the options for creating an input file for a solver (an analysis set). It can launch the NX NASTRAN solver or another solver that has been set up to run on the same PC. The analysis manager, together with VisQ, can also set up and run analyses with solvers on other PCs. The analysis sets are stored with the FEMAP model file, and can also be stored in a FEMAP library that can be accessed from different model files.
What Create the analysis set and solve the model.
How Step
UI
Command/Display
1.
Model, Analysis Menu
Tip: You can also create a new Analysis Set using the Manage command on the “context sensitive menu” located on the Analyses branch in the Model Info tree (simply click to highlight the top level of the Analyses branch or any existing Analysis Set, then right mouse click to see the context sensitive menu). 2.
Analysis Set Manager dialog box: New
3.
Analysis Set dialog box: Title: Glued Contact
4.
Analysis Program: 36..NX Nastran Analysis Type: 1..Static
32-16 Step
UI
Analysis of a Simple Assembly
Command/Display
5.
Click OK
Notice: The analysis set manager displays all analysis sets defined in the model, and the sections that make up the input file for the solver. Clicking on a plus sign will expand the tree and display individual options that can be edited by double-clicking on an option. For this analysis, you’ll use the default values for these options. 6.
Analyze
Notice: The Analysis Monitor window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results of “Glued Contact” Analysis For this example, you will display the Deformed Shape and Contour Plot of the Solid von Mises Stress.
What Display the deformed model and the Solid von Mises Stress.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
3.
Deformed and Contour Data
4.
Select PostProcessing Data dialog box: Output Set: 1..NX Nastran Case 1 In Output Vectors: Deformation: 1..Total Translation Contour: 60031..Solid Von Mises Stress
5.
OK (all dialog boxes)
Modifying the Connection Property
Step
UI
32-17
Command/Display
You can perform some other Post-processing commands on this model, then save the model. For some interesting Post-processing options for Solid Elements, such as Dynamic Cutting Plane and Dynamic Isosurface, see Example 7: Using postProcessing. At this point, we will now modify the Connection Property and add a Constraint to run the Model again using “Linear Contact” instead of “Glued Contact”. To do this, you will again access a command via a “context sensitive menu” from the Model Info tree.
Modifying the Connection Property What Modify the Connection Property using the Model Info tree.
How Step 1.
UI
Command/Display In the Model Info tree, expand the Connections branch (click on the “+” sign to the right of the title) to see the different Connection entities
32-18 2.
Analysis of a Simple Assembly
Expand the Properties branch to view the Connection Properties in the model
You will notice there is only one Connection Property in the model. You are going to modify this property and then run the analysis again. 3.
Click the right mouse button on the highlighted Connection Property. When the “context sensitive” menu appears, choose the Edit command.
4.
In the Define Connection Property dialog box: Change the Connect Type from “1..Glued” to “0..Contact”
Notice: The NX Linear tab is currently active. When you change the Connect Type from “1..Glued” to “0..Contact” certain fields are made “inactive” (greyed out) and other fields become available. In this case, we will just use the default values for “Linear Contact” in this exam 5.
Click the Defaults button at the bottom of the Define Connection Property dialog box
6.
In the Contact Pair (BCSET) section, enter the following value: Friction: 0.2
7.
Click OK
Now you will return the model to a view where another constraint can be added easily.
Modifying the Connection Property
What Display only the Geometry, Loads and Constraints in an undeformed, uncontoured plot.
How Step
UI
Command/Display
1.
View, Select Menu
2.
View Select dialog box: Deformed Style: None - Model Only Contour Style: None - Model Only
3.
4.
Click OK
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
5.
In View Quick Options dialog box: Click Analysis Entities Off button, then... Click Geometry On button, then... Click Load/Constraint On button, then... Click Done
32-19
32-20
Analysis of a Simple Assembly
Applying additional Constraints for stability You may need to place a few more constraints on the model to keep the “Pin” from sliding out of the holes in the “Baselink” and the “Plunger”.
What Create some “sliding along surface” constraints set on the two ends of the “Pin”
How Step
UI
Command/Display
1. Menu
Surfaces might still be the “Active” entity type in the Select Toolbar depending on what other post-processing you did on the Glued Contact model. If there is no “Active” entity, use the Selector Entity menu on the Select Toolbar (first icon) to select Surface. Tip: The Select Toolbar remembers the last entity type which was “Active” and a shortcut to make that entity “Active” again is to simply click the Selector Entity icon. Once you are done using the Select Toolbar, click the icon again and it will toggle back to the “no active entity” icon.
2.
Clear the Selector using the Selector Clear icon (4th icon from the left on Select Toolbar).
This will clear the Selection List. Tip: Along with clearing the entire Selection List, you can instead use the Clear Active Entity command on the Clear Selector Menu.
This will only remove the entities from the Selection List which are the same entity type as “Active” entity type in the Select Toolbar. This is very helpful if you are creating a large Selection List with many different entity types. 3.
With Surface “Active” in the Select Toolbar: Pick the surfaces at each end of the “Pin” (surfaces 41 and 42). If you turn on the Entity Info dockable pane, you will be able to see which surfaces you are choosing as you pick them. Use the Tools, Entity Info command to open up this pane. Tip: You may need to rotate the model to pick both of these surfaces. When the Select Toolbar has an “Active” entity type, you can rotate the model using by holding down the middle mouse button or wheel and then moving the mouse around.
Analyzing the “Linear Contact” Model
Step
UI
32-21
Command/Display
4.
Click the right mouse button on any of the highlighted Surfaces or anywhere in the graphics window. When the “context sensitive menu” appears, choose the Constraint command. This will bring up the Create Constraints on Surfaces dialog box.
5.
Create Constraints on Geometry dialog box: Select Surface, then... Select Sliding along Surface (Symmetry)
6.
Click OK
Note: The surfaces will NOT change color (This has been done for this example to show which surfaces to select), but the small “Selected Markers” (circles in above figure) will appear in FEMAP to let you know the surfaces have been selected. THE MODEL IS NOW READY TO BE ANALYZED!
Analyzing the “Linear Contact” Model What Analyzing the model via a “context sensitive menu” from the tree.
How Step
UI
Command/Display
1.
Model, Analysis Menu
2.
Analysis Set Manager dialog box: Click Analyze
32-22 Step
UI
Analysis of a Simple Assembly
Command/Display Tip: You can also get to an existing Analysis Set using the Manage command on the “context sensitive menu” located on the Analyses branch in the Model Info tree (simply click to highlight the top level of the Analyses branch or any existing Analysis Set, then right mouse click to see the context sensitive menu). Also, if you already have an Analysis Set created, you can simply use the Analyze command on the Analyses branch “context sensitive menu”. If you only have one analysis set, FEMAP will run it from the top-level Analyses branch. If you have multiple Analysis Sets, select an individual Analysis Set and then use the context sensitive menu to Analyze that set. Notice: The Analysis Monitor window will display the status of the solve. You’ll know that the solve is done when the Messages dockable pane tells you that cleanup of the output set is complete.
Post-processing the Results of “Linear Contact” Analysis For this example, you will again display the Deformed Shape and Contour Plot of the Solid von Mises Stress.
What Display the deformed model and the Solid von Mises Stress.
How Step
UI
Command/Display
1.
Crtl-Q
This will bring up View Quick Options dialog box:
OR Notice: The Quick Options icon appears on the View Toolbar
2.
In View Quick Options dialog box: Click All Entities Off button, then...
3.
CHECK Element box located in the Mesh section, then
4.
Click Done
5.
View, Select Menu
6.
View Select dialog box: Deformed Style: Deform Contour Style: Contour
Post-processing the Results of “Linear Contact” Analysis
Step
UI
32-23
Command/Display
7.
Deformed and Contour Data
8.
Select PostProcessing Data dialog box: Output Set: 2..NX Nastran Case 1 In Output Vectors: Deformation: 1..Total Translation Contour: 60031..Solid Von Mises Stress Notice: The displacements and stresses are quite a bit higher for the “Linear Contact”. This is because the model was allowed to move much more compared to when the model was “Glued” together.
9.
OK (all dialog boxes)
10.
Tools, Toolbars, Post (If the Post Toolbar is already visible just click the icons shown below) Menu
This will bring up the Post Toolbar.
Click the Post Options icon from the drop down list
from the Post Toolbar and select Actual Deformation
Notice: This can also be accomplished by 1. Pressing the F6 key or using the View, Options menu 2. Selecting Postprocessing as the category 3. Highlighting Deformed Style in the Options list 4. Unchecking the “% of Model (Actual)” box 5. Clicking OK It is much easier to use the Post Options menu on the Post Toolbar for this task 11.
Turn off the “Filled Edges” in the model using the View Style Menu on the View Toolbar.
Select Filled Edges from the View Style and the lines representing the elements will no longer be visible. This cleans up the view somewhat for creating pictures.
32-24 Step
UI
Analysis of a Simple Assembly
Command/Display
Again, you can perform some other Post-processing commands on this model, then save the model. For some interesting Post-processing options for Solid Elements, such as Dynamic Cutting Plane and Dynamic Isosurface, see Example 7: Using post-Processing. This is the end of the example. You don’t need to save the model file.
Index A advanced post options 7-4 analysis buckling 3-1, 32-1 analysis manager 3-11, 11-16, 12-10, 13-14, 14-12, 32-15 animation AVI 7-16 copy to other applications 7-14 speed 7-15 AutoCad file 12-1 AVI file 7-16 axisymmetric model 12-1
B beam 11-1 cross section 11-4 property 11-2 beam diagram 11-20 boundary conditions applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 boundary surface 3-3, 4-2, 8-4, 12-5, 32-13 break 4-5 buckling 3-1, 32-1
C cache pages 2-11 cleanup 9-5, 9-7 coincident nodes 3-7, 11-11, 32-15 constraint fixed 4-16, 8-10, 32-8 nodal 11-12 symmetry 4-16, 8-10, 11-12, 32-8 constraints applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 nodal 3-8, 12-7, 13-12, 32-15 on curves 14-11 symmetric 13-12 contour data 3-12, 7-1, 7-2, 12-11, 32-16 contour options 7-4 criteria data 11-17 cross section beam 11-4 display 11-7 Ctrl-Z 9-3 curve 4-4, 4-10 list 9-6 cutting plane 7-4
D deformed data 3-12, 7-1, 7-2, 11-17, 12-11, 32-16 degenerate surface 8-1
delete 13-3, 13-6, 14-4, 14-7 DXF file 12-1 Dynamic Analysis Direct Transient 15-1 Modal Frequency 16-1, 17-1 Random Response 18-1 Response Spectrum 19-1 Dynamic Analysis Parameters Direct Transient 15-7, 19-8 Modal Frequency 16-9, 17-6, 18-7 dynamic cutting plane 7-6 dynamic isosurfaces 7-6
E element beam 11-1 create 10-5 display 6-4, 11-7 fill 6-5 properties 6-4 properties and materials 3-2, 4-18, 11-2, 12-3, 32-13 rod 11-9 shrink 6-5 errors starting 2-8 explode 9-5 extrude 4-2, 4-7
F feature suppress 8-2, 8-6 file DXF 12-1 STP 14-1 X_T 8-2, 9-1, 13-1 fill 6-5 free body display 13-15, 13-17, 14-12 free edge 3-6, 10-2, 32-15, 1-1 functions 15-3
G geometry import 3-1, 4-1, 8-2, 9-1, 10-1, 11-1, 12-1, 13-1, 14-1, 32-1 meshing 3-3, 4-18, 32-13 repair 9-1 sliver 9-1 geometry mesh options 11-9 graphics copy to other applications 7-12 graphics boards 2-1 group 5-1 create 5-1, 5-3, 5-6, 10-3, 13-15 display 5-3
I-2
Index
model data 5-7, 10-3 plot 7-10 report 5-4
H hardware requirements 2-1 hidden line 6-2 hide layer 5-9
I import AutoCad DXF file 12-1 model file 5-1 neutral file 3-1, 4-1, 10-1, 11-1, 32-1 Parasolid X_T file 8-2, 9-1, 13-1 STP file 14-1 Installation PC Network 2-5 PC Stand Alone 2-1 isosurface 7-4
L layer 5-1, 5-9 view 5-9, 11-5 license file 2-5 line 4-12 loads applying 3-8, 4-16, 8-9, 12-7, 13-10, 14-10, 32-15 elemental 12-8 nodal 3-10, 11-15 on curve 13-10 on surfaces 14-10
M manual conventions 1-3 mass properties 9-2 material defining 3-2, 4-18, 11-2, 12-3, 32-13 merge nodes 11-11 mesh 4-18 curve 11-6, 11-9 repair 10-1 solid 8-7, 9-3, 9-9, 10-6 surface 3-3, 3-5, 12-5, 13-8, 14-9, 32-13 mesh attributes 13-8, 14-8 mesh size 3-4, 12-2, 13-8, 14-9, 32-15 midsurface 13-1, 14-1 create 13-4, 14-2 model import 5-1 open 6-1 model data 5-7, 6-3 model file 5-1, 6-1 model style 6-2
N network licensing 2-5 neutral file 3-1, 4-1, 10-1, 11-1, 32-1 nodes coincident 3-7, 11-11, 32-15 Nonlinear Gap Contact 26-1 Large Deformation 27-1 Plastic Deformation 25-1 Slide Line Contact 28-1 Snap Fit Contact 29-1
O open model file 6-1 output set 7-9 overview FEMAP 1-1
P Parasolid file 8-2, 9-1, 13-1 part creating 4-2 pattern 4-8 plots 7-1, 7-2 post-processing 3-12, 7-1, 11-17, 12-11, 13-15, 14-12, 32-16 pressure 12-8, 14-10 properties groups 5-6 property beam 11-2 defining 3-2, 4-18, 11-2, 12-3, 32-13
Q quick options 11-11
R RAM Management 2-11 render 6-2 report create 5-4 results 3-12, 11-17, 12-11, 13-15, 14-12, 32-16 reverse normal direction 11-8 rotate 11-6
S security device 2-2, 2-10 upgrading 2-4 show 5-5 layer 5-9 shrink 6-5 slice 8-3, 13-2 sliver geometry 9-1 software requirements 2-1 solid model
Index
analyzing 4-1 solids from elements 10-6 solving 3-11, 11-16, 12-10, 13-14, 14-12, 32-15 Starting FEMAP 2-8 Step file 14-1 stitch 9-2, 9-8, 13-7 surface degenerate 8-1 prepare for meshing 8-1 stitch 9-2 symmetry constraint 4-16, 8-10, 11-12, 13-12, 32-8
U
T
workplane 4-12
The 1-3 Thermal Analysis Enclosure Radiation 24-1 Free Convection 22-1 Steady State Heat Transfer 21-1 Temperature Dependency 23-1 Thermal Stress 20-1 trim with curve 14-5
undo 9-3 update elements 11-8
V view options 6-3 view select 6-1
W X X_T file 8-2, 9-1, 13-1 XY plot 7-7
Z zoom 11-8
I-3
I-4
Index
